Trademarks AxisVM is a registered trademark of Inter-CAD Kft.
All other trademarks are owned by their respective owners.
Inter-CAD Kft. is not affiliated with INTERCAD PTY. Ltd. of Australia.

Disclaimer The material presented in this text is for illustrative and educational purposes
only, and is not intended to be exhaustive or to apply to any particular
engineering problem for design. While reasonable efforts had been made in
the preparation of this text to assure its accuracy, Inter-CAD Kft. assumes no
liability or responsibility to any person or company for direct or indirect
damages resulting from the use of any information contained herein.

Changes Inter-CAD Kft. reserves the right to revise and improve its product as it sees fit.
This publication describes the state of this product at the time of its
publication, and may not reflect the product at all times in the future.

Version THIS IS AN INTERNATIONAL VERSION OF THE PRODUCT THAT MAY
NOT CONFORM TO CORRESPONDING STANDARDS IN A RESPECTIVE
COUNTRY AND IS AVAILABLE SOLELY ON AN “AS IS” BASIS.

Limited warranty INTER-CAD KFT. MAKES NO WARRANTY, EITHER EXPRESSED OR IM-
PLIED, INCLUDING BUT NOT LIMITED TO ANY IMPLIED WARRANTIES
OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE,
REGARDING THESE MATERIALS.
IN NO EVENT SHALL INTER-CAD KFT. BE LIABLE TO ANYONE FOR
SPECIAL, COLLATERAL, INCIDENTAL, OR CONSEQUENTIAL DAMAGES
IN CONNECTION WITH OR ARISING OUT OF PURCHASE OR USE OF
THESE MATERIALS. THE SOLE AND EXCLUSIVE LIABILITY TO INTER-
CAD KFT., REGARDLESS OF THE FORM OF ACTION, SHALL NOT EXCEED
THE PURCHASE PRICE OF THE MATERIAL DESCRIBED HEREIN.

Technical support
and services
If you have questions about installing or using the AxisVM, check this User’s
Manual first - you will find answers to most of your questions here. If you
need further assistance, please contact your software provider.

AxisVM is a finite-element program for the static, vibration, and buckling
analysis of structures. It was developed by and especially for civil engineers.
AxisVM combines powerful analysis capabilities with an easy to use graphical
user interface.

Postprocessing Displaying the results: deformed/undeformed shape display; diagram, and iso-
line/surface plots; animation; customizable tabular reports.
After your analysis, AxisVM provides powerful visualization tools that let you
quickly interpret your results, and numerical tools to search, report, and per-
form further calculations using those results. The results can be used to display
the deformed or animated shape of your geometry or the isoline/surface plots.
AxisVM can linearly combine or envelope the results.

Documentation Documentation is always part of the analysis, and a graphical user interface
enhances the process and simplifies the effort. AxisVM provides direct, high
quality printing of both text and graphics data to document your model and
results. In addition data and graphics can be easily exported (DXF, BMP, JPG,
WMF, EMF, RTF, HTML, TXT, DBF).

If available RAM exceeds 2 GB, the limit of 2 GB per application can be in-
creased to 3 GB by editing C:\boot.ini. Enter the /3GB switch this way:
[boot loader]
timeout=30
default=multi(0)disk(0)rdisk(0)partition(1)\WINNT
[operating systems]
multi(0)disk(0)rdisk(0)partition(1)\WINNT="????" /3GB
where ???? stands for the full name of the operating system.

14 AxisVM 8+Release 4

2.2. Installation
Software
Protection

F
The program is protected by a hardware key. Two types of key are available:
parallel port (LPT) keys and USB keys.
Plug the key only after installation is complete, because certain operating sys-
tems try to recognize the plugged device and this process may interfere with the
driver installation.
Windows 98 requires a special driver to handle the USB port. For want of this
driver the USB key does not operate.
Windows NT must have Service Pack 3 or higher installed on the system to reach
the key properly. Non-network drivers will be automatically installed.
If you encountered problems you can install this driver later from the CD.
Run the Startup program and select Reinstall driver .
Standard Key First install the program then plug the key into the computer.

Network Keys If you have a network version you must install the network key. In most cases
AxisVM and the key are on different computers but to make the key available
through the network the Sentinel driver must be installed on both computers.
AxisVM Version 8+ is shipped with a parallel port or USB Sentinel Super Pro
dongle but earlier customers may have parallel port NetSentinel dongle.
a. Sentinel SuperPro dongle
1. Insert the AxisVM CD in the CD-ROM drive of the AxisVM server.
Run [CD Drive]: \ Startup.exe. Select Reinstall driver. This type of
network key requires at least a 7.1 driver. CD contains the 7.3 version of
the driver.
2. Connect the key to the parallel or USB port of one of the computers.
This way you select the AxisVM server.
F
To run AxisVM on any computer on the network SuperPro Server must be
running on the server. If it stops all running AxisVM programs stop.
b. NetSentinel dongle
1. Insert the AxisVM CD in the CD-ROM drive of the AxisVM server.
Run [CD Drive]: \ Sentinel \ English \ Driver\ setup.exe to install
Sentinel driver.
2. Connect the key to the parallel port of one of the computers. This way
you select the AxisVM server.
3. Copy the contents of the folder [CD Drive]: \ Sentinel \ English \ server
\ Disk1 \ Win32 to a folder of the server’s hard drive.
4. Run NSRVGX.EXE from that folder. This server program handles the
network key and communicates with the applications on the network.
F
To run AxisVM on any computer on the network NSRVGX must be running on
the server. If NSRVGX stops all running AxisVM programs stop.
Installation

AxisVM runs on Windows 98 / NT / 2000 / XP / Vista operating systems.
Insert the AxisVM CD into the CD drive. The Startup program starts
automatically if the autoplay option is enabled. If Autoplay is not enabled, click
the Start button, and select Run.... Open the Startup.exe program on your
AxisVM CD. Select AxisVM 8 Setup and follow the instructions.

F
If the setup program cannot be launched or the following message appears:
AUTOEXEC.NT - The system file is not suitable for running MS-DOS and Microsoft
Windows applications, a Windows system file must be missing.

Installation under Vista Operating System:
• You need the latest Sentinel driver. You can download it:
www.axisvm.eu /Support- Service Pack for AxisVM 8+
• Click on the program icon with the Mouse right button after the
installation of AxisVM program
• Choose the Properties menu item from the Quick Menu.
• Select the Compatibility tab on the appearing dialog and turn on the
Run as administrator checkbox.

User’s Manual 15

By default the program and the example models will be installed on drive C: in
C:\Program Files\AxisVM8
and
C:\Program Files\AxisVM8\Examples
folders. You can specify the drive and the folders during the installation
process. The setup program creates the AxisVM program group that includes
the AxisVM application icon.

Starting AxisVM

Click the Start button, select Programs, AxisVM folder, and click the AxisVM8
icon. At startup a splash screen is displayed (see... 3.6.4 About) then a welcome
screen is shown where you can select a previous model or start a new one.
Clearing the checkbox at the bottom turns the welcome screen off for
the future. To turn it on choose the Settings\Preferences\Data Integrity dialog and
check the Show welcome screen on strartup checkbox.

F
If you have an older version of Windows and Internet Explorer some toolbar
icons may disappear. Then you have to update your Windows by running
[CD Drive]:\Comctl32\401comupd.exe.

Upgrading It is recommended to install the new version to a new folder. This way the
previous version will remain available.

Converting earlier
models
Models created in a previous versions are recognized and converted
automatically. Saving files will use the latest format by default. Saving files in
the file format of one of the previous versions (5.0, 6.0, 7.0) is possible but this
way the information specific to the newer versions will be lost.

* If beams or/and ribs are in the structure
2.3. Getting Started
Step-by-step input schemes are presented in the Section 7. See Example 1
of Chapter 8 with a step-by-step input scheme in 7.2 Plane Frame Model

There are three major steps in a modeling process:
Geometry The first step is to create the geometry model of the structure (in 2D or 3D).

Elements In the second step you must specify material and element properties, mesh the
geometry into elements (assigning the properties and a mesh, to the wire-
frame model), and define the support conditions.

Loads

In the third step you must apply different loads on the model.
The end result will be a finite element model of the structure.
Once the model is created it is ready for analysis.
In Chapter 7, the step-by-step modeling of a few typical structures are
presented. The following types of structures are shown:
1. Plane truss girder
2. Plane frame
3. Plate structure
4. Membrane cantilever
5. Seismic analysis

Understanding of these simple models will allow you to easily build more
complex models.
It is recommended that you read the entire User’s Manual at least once while
exploring AxisVM.
In chapter 1 you can find the timely, new features of the version.
Chapter 2 contains general information about using AxisVM. In other chapters
the explanation follows the pre- and postprocessor menu structures.
Please consult this User’s Manual every time you are using AxisVM.

User’s Manual 17

2.4. AxisVM User Interface
This section describes the working environment of the full AxisVM graphical
user interface. Please read these instructions carefully. Your knowledge of the
program increases the modeling speed and productivity.

AxisVM screen After you start AxisVM a screen similar to the following picture appears:

The parts of the AxisVM screen are briefly described below.
Graphics area The area on the screen where you create your model.
Graphics cursor The screen cursor is used to draw, select entities, and pick from menus and
dialog boxes. Depending on the current state of AxisVM, it can appear as
a pick-box, crosshairs with pick-box, or pointer.
Top menu bar Each item of the top menu bar has its own dropdown menu list. To use the top
menu bar, move the cursor up to the menu bar. The cursor will change to
a pointer. To select a menu bar item, move the pointer over it, and press the
pick button to select the item. Its associated sub-menu will appear.
Active icon The active icon represents the command that is currently selected.
Icon bar The icons represent working tools in a pictorial form. These tools are accessible
during any stage of work. The icon bar and flyout toolbars are draggable and
dockable.
Coordinate window The window on the graphics area displaying the graphics cursor coordinates.

Color legend
window
The window shows the color legend used in the display of the results.
Appears only in the post-processing session.

Info window The window shows the status of the model and results display.

Context sensitive
help
Provides a help message that depends on the topic under process.

The model With AxisVM you can create and analyze finite element models of civil
engineering structures. Thus the program operates on a model that is an
approximate of the actual structure.
To each model you must assign a name. That name will be used as a file name
when it is saved. You may assign only names that are valid Windows file
names. The model consists of all data that you specify using AxisVM.
The model’s data are stored in two files: the input data in the filename.axs
and the results in the filename.axe file.
AxisVM checks if AXS and AXE files belong to the same version of the model.

2.5. Using the Cursor, the Keyboard, the Mouse
Graphics cursor

As you move your mouse, the graphics cursor symbol tracks the movement on
the screen. To select an entity, an icon or menu item, move the cursor over it
and click the left mouse button. The shape of the cursor will change
accordingly (See... 4.7.1 Cursor Identification), and will appear on the screen
in one of the following forms:

Crosshairs: Pointer: Crosshairs/zoom mode:

If you pick an entity when the cursor is in its default mode (info mode), the
properties of that entity will be displayed as a tool tip. Depending on the menu
your cursor is on, you may get the properties of the following entities:

The keyboard You can also use the keyboard to move the cursor:
Arrow keys, 8
Moves the graphics cursor in the current plane.

[Ctrl] +
Arrow keys, 8
Moves the graphics cursor in the current plane with a step size
enlarged/reduced by a factor set in the Settings dialog box.

[Shift]+
[↑][↓][←][→],8
Moves the graphics cursor in the current plane on a line of angle n·∆α , custom
α or α +n·90°.

[Home] [End] Moves the graphics cursor perpendicular to the current plane.

[Ctrl]+
[Home], [End]
Moves the graphics cursor perpendicular to the current plane with a step size
enlarged/reduced by a factor set in the Settings dialog box.

[Esc] or 8
right button
Interrupts the command and/or returns to an upper menu level.

[Enter]+[Space] 8
left button
Selects an item from a menu, executes a command, and selects entities.
These are termed command buttons.

[Alt] Activates the main menu

[Tab] Moves the focus from control to control in a dialog.

User’s Manual 19

[+] [-]

Performs fast zoom in/out and pan. The zoom and pan parameters are defined
by the current position of the graphics cursor in the graphics area, and by the
magnification factor set in Settings / Options / Zoom Factor. Center of the fast
zoom in/out is always the current graphics cursor position.

[Insert]
or [Alt]+[Shift]
Moves the relative origin (i.e. the reference point of the relative coordinates) to
the current graphics cursor position.

8 wheel
Roll forward to zoom in
Roll backwards to zoom out
Press the wheel and drag to drag the drawing area
Centre of zoom in and zoom out is the current position of the cursor.

2.7. Quick Menu
8 right button
When the cursor is over the graphics area, by pressing the right mouse button
a quick menu appears in accord with the current command in use.
Selection Geometry / Elements / Loads Results

2.8. Dialog Boxes
After selecting a function usually a dialog box appears on the screen. These
dialog boxes can be used the same way as any other Windows dialog.
The dialog font can be changed by selecting the Settings\Preferences\Fonts dialog
and clicking the font sample label Dialog boxes.
You can change the position of all dialog windows. The program saves the
latest position and displays the dialog on the same position next time.

2.9. Table Browser
[F12]
AxisVM uses tables to display numerical information on the screen allowing
changes in formatting. The tables operate in the same way independent of the
content displayed. All the tables AxisVM creates are available through the
Table Browser dialog box by clicking its button or pressing [F12].

The model data to be displayed in the Table Browser can be selected from the
tree structure in the left side of the browser. If you use Table Browser while
working in the pre-processor, input model data is displayed only. While
working in the post-processor, the model results are also displayed.
F
Only the data of the current selection (if any) or of the active (i.e. displayed) part
is listed by default.
User’s Manual 21

The tree view on the left lists element / load data, result tables and libraries in a
hierarchy and can also be used as a model overview.

Using the table A table can contain more rows and/or columns than can be displayed at the
same time. It can be viewed in its entirety using the scroll bars and/or using the
keyboard as follows:

Arrow keys
8 left button
Moves the edit focus up and down, to the left and to the right, and scrolls the
table along the rows or columns. Clicking an editable cell moves the edit focus
to that cell.

[Home] Moves the focus to the first cell of the row.

[End] Moves the focus to the last cell of the row.

[Ctrl]+[Home] Moves the focus to the first cell of the first row

[Ctrl]+[End] Moves the focus to the last cell of the last row.

[Page Up] Displays the previous page of rows.

[Page Down] Displays the next page of rows.

[Ctrl]+ [→] Moves the focus to the next (to the right) page of columns (only in tables
where more columns can be displayed at the same time).

[Ctrl]+ [←] Moves the focus to the previous (to the left) page of columns (only in tables
where more columns can be displayed at the same time).

[Enter] Ends the current editing in the edit box storing the data entered and moves
the edit box a column to the right or to the first column of the next row.

[Esc]
8 right button
Aborts the current editing in the edit box.

[Shift] While the [Shift] key is down all direction keys will select cells instead of
moving the edit focus. You can also select cells by dragging the mouse.
Clicking a fixed (topmost) cell of a column selects the column. Clicking a fixed
(leftmost) cell of a row selects the row. Clicking the top left cell selects the
entire table. Selected cells can be copied to clipboard as a table. If selection is
within an editable column you can set a common value for the selected cells.
See... Set Common Value below

Browse Library
, [Ctrl]+ [L]
Loads cross-sectional or material data from a library. You can also save the
current content of the table in a custom library.

Import DBase File

Imports a DBase file name.dbf into the current table. The program checks the
values of the fields and sends an error message if an incompatible value is
found.

Save As DBase File

Exports the current table into a Dbase file name.dbf. The field names are
generated based on the names of the columns. The fields will be of text type.

Save As HTML

Exports the current table into an HTML file name.htm. This file can be imported
as a table into Word or can be opened in web browser applications. Some
formatting information of the columns will be lost.

Save As TXT

Exports the current table into a TXT (ASCII) file name.txt.

Save As RTF

Exports the current table into an RTF file name.rtf using the current template
file. You can import this file into Microsoft Word or any other word processor
which can import RTF files. See... 2.10.1 Report

New Cross-Section
Table
Creates a new cross-section data file name.sec. The table created will be placed
together with the cross-sections of the same type.
You can store cross sections of any type in these tables. Type of the table
determines only the position of the table in the Cross-section Library.

Print
, [Ctrl]+ [P]
Prints all the information displayed in the table to the selected printer or to a
file, with the page header and comment row previously set with the File/Header
menu command.

Exit
[Alt]+ [F4]
Exits the table in the same way as the Cancel button (the changes are not
saved).

Edit

User’s Manual 23

New
[Ctrl]+ [Insert]
Adds a new row to the list, and allows you to fill all the editable cells with data
in a fixed order from left to right.

Delete
[Ctrl]+ [Del]
Deletes the selected rows.

Select Table
[Ctrl]+ [A]
Selects the entire table. Clicking the top left cell does the same.

Design New
Custom Cross-
section
[Ctrl]+[G]
Starts the graphics Cross-Section Editor, allowing the input of a new custom
cross-section.

Modify Custom
Cross-section
[Ctrl]+[M]
Starts the graphics Cross-Section Editor, allowing the modification of a custom
cross-section previously created with the graphics Cross-Section Editor.

Automatic cross-
section shape update
If this function is on changing section parameters in the table leads to the re-
calculation of geometry and cross-section parameters.

Delete unused
cross-sections
Unused cross-sections will be deleted from the table.

Copy
[Ctrl]+ [C]
Copies selected cells to the Clipboard as a table.

Paste
[Ctrl]+ [V]
Pastes table cells from the Clipboard overwriting cell values.
If any of the values is unacceptable Paste aborts.
If entire rows were cut or copied and the table allows inserting new rows you
can also add clipboard data to the end of the table instead of overwriting the
existing rows.

Set Common Value Sets a common value for the selected cells within a column.
Example: you can set the Z coordinate of all nodes to the same value making
the model absolutely flat.
Available from the Table Browser Menu / Edit / Set Common Value.

Go to
[F5]
Jumps to a specified row in the table.

Format
Defining data

Column Formats

[Ctrl]+ [Alt]+ [F]

You can specify whether a column is visible or not, by setting the check boxes
of the corresponding columns.
The display format is set according to the settings in the Units/Settings
dialogue window (see...3.3.6 Units and Formats).
Many cells require the entry of a numeric value. When entering real numbers
you can use the following characters:
+ - 0 1 2 3 4 5 6 7 8 9 0 E
and the standard Windows decimal separator specified in Start / Settings /
Control Panel / Regional Settings / Number / Decimal symbol field.
In some cases you cannot enter a negative number so the - key is deactivated
while entering these kind of values. If an integer value is required you cannot
use the decimal separator and E.

The cross-names which are signed by bold letter will remain in the table if the
Delete Unused Cross-sections switch is turned on. See… Edit menu item.

In case of result query new items appear on the Format menu and the Toolbar.

Result query

Result Display
Options
[Ctrl]+[R]
You can control finding the extremes for result components and set to show
results (Result) and/or just the extremes (Extremes).
See in detail: 6.1.4 Result Tables

Results On/Off
[Ctrl]+[T]
Display of results can be turned on / off.

Extremes On/Off
[Ctrl]+[E]
Display of extremes can be turned on / off.
Order of load cases... The display order of load cases can be customized.
See... 4.10.1 Load Cases, Load Groups

Property Filtering
[CTRL]+[Q]

Property filtering helps you to select which elements to include in the table.

Report

Current report You can set the current report. Tables will be added to this report.
See...2.10 Report Maker.

Add table to report
[F9]
Adds the current table to the current report. If the selected node in the
treeview has sub-nodes (e.g. MODEL or Loads) all tables under that node will
be added. If the current table is a result table and is set to display extremes
only all sub-tables will display extremes only. See... 2.10 Report Maker.

Report Maker
[F10]
Opens Report Maker.

User’s Manual 25

Help

About Table Displays info about the table.

About Table
Browser
Displays info about the table browser operation.

OK Saves the data and closes the table.

Cancel Closes the table without saving the data.

F
Result tables also display the extremes (minimum and maximum values) of the
data if you select this option in the Display Options dialog when you enter
Table Browser. Displaying both the individual values and the extremes is the
default setting.

2.10. Report Maker
[F10]
Report Maker is a tool to compile a full report of a project using report items
(tables/drawings/pictures created by AxisVM and user-defined text blocks).
Reports are stored in the model file (*.axs) and can be printed or saved as a
Rich Text Format (RTF) file. RTF files can be processed by other programs
(e.g. Microsoft Word).

Tables exported from Table Browser are automatically updated if the model
has been changed or some of its parts were deleted.
Report Maker can handle several different reports for the same project.
The structure of reports is displayed in a tree view on the left. The properties
of the selected report item are shown on the right side of the window.

26 AxisVM 8+Release 4

Table If a table is selected, its comment text, column titles and other properties are
shown. Display of title, comment and columns can be turned on and off.

Text If a text block is selected the text is shown on the right. Click the button
Edit text... to make changes.

Picture or Drawing If a picture or drawing is selected it is shown on the right. Its size, alignment
and caption can be set.

Drawings Library By clicking the Drawings Library tab you can browse the saved drawings and
add the selected ones to the report. Unlike the pictures in the Gallery these
drawings are not graphics files, but view settings stored to recreate the
drawing at any time. This way drawings will be automatically updated if we
change and recalculate the model. See in detail... 3.5.7 Drawings Library,
3.5.8 Save to Drawings Library.

Gallery By clicking the Gallery tab you can browse the saved pictures (BMP, JPG,
WMF, EMF) located in a folder named Images_modelname and add the selected
ones to the report. This folder is automatically created as a subfolder of the
model folder. See in detail... 2.10.4 Gallery

You can save the current drawing on screen or the result tables in design
modules with the function of Edit\ Saving drawings and design result tables
in main menu. See... 3.2.8 Saving drawings and design result tables

One or more selected pictures in the Gallery can be inserted into a report
by selecting menu item Gallery/Add pictures to the report or clicking the arrow
button above the Gallery or by drag and drop.
In printed reports Report Maker automatically builds a table of contents and
inserts it to the beginning of the report. Tables are listed according to their
titles. Text blocks are listed only if they were formatted using one of the
Heading styles in the Text Editor. Pictures are listed only if they have
a caption.

User’s Manual 27

2.10.1. Report

New report

Creates a new report. Report names can be 32 characters long.

Delete entire report

[Del], [Ctrl]+[Del]
Deletes the current report (i.e. the report which contains the selected item).
Pictures used in the report are not deleted from Gallery.

Rename Gives a new name to an existing report.

Save As TXT Exports the report into a ASCII text file. Drawings or pictures are not included.

Export as RTF

Saves the report as name.rtf using the current template. If you save the file to a
folder different from the model folder all picture files used in the report are
copied to an automatically created subfolder Images_modelname. It is necessary
because pictures are only linked and not saved into the RTF document.
To print the RTF report on a different machine make sure that picture files are
also copied to a subfolder Images_modelname.
Character and paragraph formatting of text blocks will be exported. The only
exception is the character color. Tables will be exported as RTF tables. Table
titles are formatted with Heading 3 style so it is easy to build a table of contents
automatically using Microsoft Word. In Insert / Index and Tables or Insert /
Reference / Index and Tables select the Table Of Contents tab of the dialog,
set Formats to From template and Show levels to at least 3.

RTF Options AxisVM saves reports to RTF files
using a template (the default one is
Template.rtf in the program folder).
You can use other templates as
well. When changing a template
you can create your own cover
sheet and header/footer for the
report. Read the text of the
template file carefully before
changing it.

Format of drawings in RTF file can also be set. Embedded WMF: Drawings are
embedded into the file. It improves portability but can result in huge file size.

Link to BMP, JPG: This option keeps the RTF file smaller as drawings are
stored in external files. Drawings appear only if pictures are located in an
Images_modelname subfolder relative to the folder of the RTF file.
Gridlines of exported tables can also be turned on/off.

Report preview
[F3]
Displays a print preview dialog. You can set the zoom factor between 10% and
500% (Page Width and Full Page is also an option). Click the buttons or use the
keyboard to move backward and forward between pages ([Home] = first page,
[PgUp] = previous page, [PgDown] = next page, [End] = last page.

Print
[Ctrl]+[P]
A dialog to set printing parameters and print a report. The options are the
same as the table printing options.

Exit Quits the Report Maker.
28 AxisVM 8+Release 4

2.10.2. Edit

Some of the functions in the Edit menu are also available in the popup menu
after clicking right mouse button on a report item.

Undo Undoes the effect of the previous command.

Redo Executes the command which was undone.

Report Builder

Report Builder creates complete structured reports based on several filter
options set on the Filter tab. Load cases, result components, parts, element and
load types can be selected and set the display of extremes or results in the
tables.
The rules of creating reports can be set on the Preferences tab. You can choose
if you want to see different element types listed within a part or different parts
listed within an element type, or if you want to see result components listed
within a load case or load cases listed within a result component.
If we imported an architectural model it is also possible to filter for
architectural objects and ask for separate tables for each architectural object.
The number of expanded levels (1-7) of the report tree on the right can be set
with the level-adjustment bar.
The tree on the right side shows the report built using the criteria set in the
left. Each report item can be turned on/off individually. The report sent to the
report maker will contain the checked items only.

Filter

User’s Manual 29

Preferences

Insert folder

Inserts a new folder into the tree, below the current item. The current folder
name appears on the right side under the folder icon.
The number of expanded levels (1-7) of the report tree can be set with the
level-adjustment bar.

Insert text into
report
[Ctrl]+[T]
Starts a built-in Text Editor to create a new text block. The formatted text will
be inserted after the selected report item.

Page break

[Ctrl]+[Alt]+[B]
Inserts a page break after the selected report item.

Move up/down
selected report item

Moves up/down the selected report item by one.

Move to / Copy to Moves / copies the selected report item to the end of another report.

Select subitems
automatically
If you turn this checkbox on and select a folder all subitems will be selected
automatically.

Deselect all Deselects all selected items in the documentation.

Select all items of
the current report
Every report item of the current report will be selected.

Delete

[Del], [Ctrl]+[Del]
Deletes the selected report item (text block, picture, table, page break).
If the current selection in the tree is a report it deletes the entire report.

Delete all report
items
Deletes all items from the current report but does not delete the report itself.

30 AxisVM 8+Release 4

2.10.3. Drawings

Add drawings to the
report
Inserts the selected drawing(s) from the Drawings Library into the selected
report. Place of insertion is determined by the selected item of the report tree.
Effect of this function is the same as that of the button on the Drawings
Library tab.

[Ctrl]+[R]
Displays a print preview of the current report.
See... 2.10.1 Report

[Ctrl]+[W]
Exports the current report to an RTF file.
See... 2.10.1 Report

[Ctrl]+[P]
Print
See... 2.10.1 Report

[Ctrl]+[Z]
Undo
See... 2.10.2 Edit

[Shift]+[Ctrl]+[Z]
Redo
See... 2.10.2 Edit

2.10.6. Gallery and Drawings Library Toolbars
You can perform certain tasks faster using these small toolbars.

Deletes selected pictures or drawings from the Gallery/Drawings Library.

Inserts selected pictures or drawings into the current report.
Place of the insertation is determined by the selected item in the report tree.

Copies pictures from other locations to the Gallery. This function is not
available on the Drawings Library tab.

2.10.7. Text Editor
After selecting Insert text to report a formatted text can be created in a simple
WordPad-like text processor.
File
Open
[Ctrl]+[O]
The main purpose of this function is to load a Rich Text file written in Text
Editor. If you open an RTF file created in another word processor it may con-
tain special commands (e.g. tables, paragraph borders, Unicode characters)
which are not supported this simple editor. As a result you may get a series of
rtf control commands instead of formatted text.

Left justify
[Ctrl]+[L]
Justifies the selected paragraphs to the left.
Centered
[Ctrl]+[E]
Justifies the selected paragraphs to the centerline.
Right justify
[Ctrl]+[R]
Justifies the selected paragraphs to the right.
Bullet
[Ctrl]+[Alt]+[U]
Places bullets before the selected paragraphs.

2.11. Redraw

Pressing this button you can make the screen redraw.
2.12. Layer Manager

If you choose Workplanes, Dimensioning - Model info a dialog will appear.
Dragging and
docking the Icon bar
and the flyout
toolbars
The left-side icon bar and any flyout toolbar can be dragged and docked.

Dragging and docking of the Icon bar
If you move the mouse over the handle of the Icon bar (on its top edge), the
cursor will change its shape (moving). You can drag the Icon bar to any
position on the screen. If you drag the Icon bar out of the working area
through its top or bottom edge the Icon bar becomes horiozontal. If you drag it
to the left or right edge it becomes vertical.
If the Icon bar is horizontal you can dock it at the top or at the bottom. You can
change the position and the order of docked toolbars by dragging. In the
Cross-Section Editor and in Beam and Coumn Reinforcement dialogs the Icon
bar cannot be docked. Closing a floating Icon bar restores its original position
docked on the left.

Dragging and docking of flyout toolbars
You can also separate flyout toolbars from the Icon bar by dragging their
handle. Closing or dragging them back to the Icon bar restores their original
position. Floating flyout toolbars can be docked at the top or at the bottom.

F
The Icon bar and the flyout toolbars can be restored to their original position by
selecting Settings\Toolbars to default position from the menu

34 AxisVM 8+Release 4

2.15.1. Selection

Activates the selection mode and displays the selection icon’s bar.

Lets you select a set of entities (nodes (points), lines, finite elements and loads)
for processing. When you execute commands you can use the Selection icon
to specify the entity set to which to apply the command to. If the Parts check
box (See section 2.15.10 Parts) is enabled the selection will refer only to the
active (visible) parts.
You can change the view settings or continue selection in another window
pane during the selection process. These allow you to select elements in the
most convenient view. The selected entities are displayed in magenta in the
graphics area.
The selection process is considered finished when the OK button is pressed.

Selection methods with selection frame:

- dragging the selection frame from left to right selects elements entirely within
the frame
- dragging the selection frame from right to left selects elements which are not
entirely outside the frame

Select

Adds the currently selected entities to the set of selected entities.
Deselect

Removes the currently selected entities from the set of selected entities.
Invert

Inverts the currently selected entities’ selection status.
All

Applies the current selection mode (add, remove, or invert) to all filtered
entities.
Previous

Restores the previous selection set.
Selection of parts

Clicking the button and a part from the list will select elements of the chosen
part.
Filter

Selects entities using different methods (selection shapes). Rectangular,
skewed rectangular, sectorial or ring selection shapes are available. In the
followings examples of the application of various selection shapes are
provided:

Selection: Result:

Rectangular

Skewed rectang.

Polyline

Sectorial

Annular

Intersected lines

OK Ends the selection, retaining the selected set for use.

Cancel Ends the selection, discarding the selected set.

F
If an entity is hidden by another entity you cannot select it by simply clicking on
it. In such a case, you have to change view to select it.
36 AxisVM 8+Release 4

$

The selected nodes are marked with a surrounding magenta rectangle. Some-
times it is necessary to double-select nodes. In this case these nodes are marked
with an additional blue rectangle surrounding them.

Selections can also be made, without using the Selection Icon Bar. Pressing and
holding the [Shift] button while selecting with the 8 will add entities to the
selection and pressing and holding the [Ctrl] button while selecting with the 8
will remove entities from the selection.
Double selections can be made by pressing and holding the [Alt] button while
double clicking on the entities with the 8.

F
During the selection we can modify the apperiance of the structure, we can
switch over an other view or perspective observation.

2.15.2. Zoom

Displays the zoom icon bar.

Zoom in

Displays an area of the model
drawing specified by two points (two
opposite corners) on the graphics
area defining a rectangular zoom
region. As a result, the apparent size
of the model displayed in the
graphics area increases.

Zoom out

Displays the model drawing from the
graphics area on the area specified by
two points (two opposite corners) de-
fining a rectangular zoom region. As
a result, the apparent size of the
model displayed in the graphics area
decreases.

Zoom to fit

Scales the drawing of the model to fit the graphics area, so you can view the
entire model.

Pan

Moves the drawing. Press and hold the left button of the 8 while moving the
mouse, until the desired position of the drawing is obtained on the screen.
Quick Drag:

You can use the mid mouse button to drag the model drawing at any time
(without the the Pan icon).
1. Click the Pan icon.
2. Drag the model to its new position.

$
This cursor shape indicates that you can pan the model.

User’s Manual 37

Rotate

After clicking this icon you can rotate the model around the centre of the
encapsulating block of the model by dragging. During the rotation the follo-
wing pet palette appears at the lower part of the screen:

Rotation methods in the order of icons:

Free rotation around the horizontal axis of the screen and the global Z axis.
Rotation around the global Z axis.
Rotation around the vertical axis of the screen.
Rotation around the horizontal axis of the screen.
Rotation around an axis perpendicular to the screen.

$
This cursor shape indicates that you can rotate the model.

Undo view
/ Redo view

Undoes / redoes the action of up to 50 view commands.

2.15.3. Views

Displays the projection of the model on the X-Z plane (front view).

Displays the projection of the model on the X-Y plane (top view).

Displays the projection of the model on the Y-Z plane (side view).

Perspective
Toolbar

Sets the parameters of the perspective display. The proper view can be set by
rotating the model drawing around the three axes, and by setting the
observation distance. Rotation angles can be set with a precision of 0.1 degrees.
You can assign a name to each setting that you want to save for later use.
Type a name into the combo and click on the icon on the left of the combo to
save the settings. To delete a perspective setting choose it from the dropdown
list and click on the Delete icon on the right side of the combo.

Observation
distance
Observation distance is the distance between the viewpoint and the centre of
the encapsulating block of the model.

Rotation

After clicking on the rotate icon a pet palette
appears as described earlier (Zoom\Rotate).

Rotate about the
horizontal axis
Rotate about the
vertical axis
Rotate about the
perpendicular axis

Displays three projection views and the perspective view of the model, and
allows you select the view that you want to display. Click the view you want to
select.

2.15.4. Workplanes

Workplanes (user coordinate systems) makes it easier to draw on oblique
planes. Consider a hole for a skylight on an oblique plane of a roof. The plane
of the roof can act as a workplane so drawing can be performed in two
dimensions. In case of workplanes altitudinal coordinate means the distance
along the axis normal to the workplane.

F
All drawing/editing functions are available in workplane mode.
Using multi-window mode a different workplane can be set for each window.

Global X-Y,
Global X-Z,
Global Y-Z
workplanes
These workplanes are parallel with
a global coordinate plane so their
position is defined by a single
coordinate. Useful when drawing
stories of a building.
General workplanes These workplanes are defined by
an origin and two vectors for the
local x and y axes.
Smart workplanes These workplanes follow the local
system of a truss, beam, rib or
domain. The origin is the first point
of the element, local x and y axes
are parallel to the local x and y axes
of the local system of the element.

F
Changing the local system of the finite element the workplane is also changing.
Deleting the finite element you delete the workplane as well.

Clicking the workplane speed button the workplane can be selected from a list.
Workplanes are also available from the main menu by selecting View \ Work-
planes or from the popup menu by selecting Workplanes.

Display options A workplane can be displayed in the global coordinate system or in its local
system.
After checking Hide elements not in the workplane only those elements are disp-
layed that are in the workplane. After checking Show elements out of workplane
grayed elements out of the workplane appears grayed.

User’s Manual 39

Changing workplane
parameters
If you select a workplane from the tree, its parameters are displayed. Editing
them and clicking the OK button or selecting another workplane will change
the parameters of the selected workplane.

Makes multiple copies of, or
moves the selected geometric
entities or loads, by translation
along a vector. You must spe-
cify the translation vector
(dX, dY, dZ), and the number
of copies (N).

Translation options Incremental: makes N copies
of the selected entities by the
distance dX, dY, dZ.
Distribute: makes N copies of
the selected entities along the
distance dX, dY, dZ (by dX/N,
dY/N, dZ/N increments).
Spread by distance: makes
copies of the selected entities
spread by distance d in the
direction of the translation
vector.
The number of copies depends on how many copies will fit into the length
defined by the translation vector dX, dY, dZ.

Nodes to connect You can select nodes that will be connected by lines to its corresponding
copies. You can choose one of the following options:

None: No nodes will be connected.

Double selected: Holding the [Alt] key pressed you can double select nodes.
These nodes will be connected.

All: All nodes to be copied will be connected.

Switches
Copy options Copy elements: You can specify the finite elements assigned to the geometric
entities to be copied as well.

Copy loads: You can specify the loads assigned to the geometric entities to be
copied as well.
F
Loads can be copied separately (without the elements).

Copy nodal masses: You can specify the nodal masses to the geometric entities
to be copied as well.

Copy dimension lines: The dimension lines will be copied only if the nodes to
which they are assigned are selected.
40 AxisVM 8+Release 4

With guidelines All rulers will also be moved (useful when moving the entire model).

With DXF layer With this option checked the transformations will be performed on the objects
of the DXF layer as well.

Visible layers only With this option checked only the visible layers will be transformed.

Steps of
translating
The translation consists of the following steps:
1. Click on the Translate icon
2. Select the entities or loads to be copied
3. Click OK on the Selection Window (or Cancel to interrupt the selection
and translation commands)
4. Select your options from within the Translate Window.
5. Click OK
6. Specify the translation vector by its start and end point

The command can be applied in the 2-3-1-4-5-6 sequence as well.

F
If you have repetitive parts in your model, you should first create these (includ-
ing the definition of finite elements, support conditions, loads, and dimension
lines), and then make copies of them.
You can use any existing point when you have to specify the translation vector.
Selected loads can be copied or moved to another load case if load case is changed
to the target load case during the operation.

2.15.5.2. Rotate
Rotation

Makes multiple copies of, or
moves the selected geomet-
ric entities or loads, by rota-
tion around a center. In X-Y,
X-Z or Y-Z views the rota-
tion axis is normal to the
current view plane. In pers-
pective view rotation axis is
always the Z axis.

You can specify the method
of rotation. Parameters de-
pend on the method: rota-
tion angle α, the number of
copies (N) and an additional
translation h along the rota-
tion axis (each copy will be
shifted by this distance).
Click the rotation center
(OX, OY, OZ), the rotation
arc start point and draw the
cursor angle.

Spread by angle: makes copies of the selected entities spread by a given angle
α specified in the dialog. The number of copies depends on how many
copies will fit into the cursor angle.

Consecutive: makes N consecutive copies of the selected entities at different
cursor angles.

Move: moves the selected entities by the cursor angle.

User’s Manual 41

Nodes to connect See... 2.15.5.1 Translate

Switches See... 2.15.5.1 Translate

In perspective view, the centerpoint, start point and endpoint can be specified
only using existing points or other identified 3D locations (i.e. a point on a
line). In perspective view, cursor angle is determined by the global X and Y
coordinates only.

2.15.5.3. Mirror
Mirror

Makes a copy of, or moves
the selected geometric enti-
ties or loads, by mirroring.
Specify two points of the
symmetry plane. The sym-
metry plane is always pa-
rallel to a global axis de-
pending on what view you
are in.

Mirror options Copy: reflects a copy of the
selected entities over the
mirror plane.
Multiple: makes consecutive
copies of the selected entities
over different mirror planes.
Move: moves the selected
entities across the mirror
plane.

Nodes to connect See... 2.15.5.1 Translate

Switches See... 2.15.5.1 Translate

In perspective view, the mirroring is possible only across a plane parallel with
the global Z axis.
2.15.5.4. Scale
Scale

Makes multiple copies of, or moves the selected geometric entities, by scaling
from a center. You must specify the scaling center, a point of reference and its
new position after scaling (coordinate ratios will determine the scaling factors).

Rendered : Displays a rendered model drawing. The line
elements are displayed with their actual cross-section and
the surface elements with their actual thickness.
The elements colors are displayed corresponding to colors
assigned to their materials. Rendered view is smoother and
shows the details of thin-walled cross-sections.

In View / Rendering options... transparency of element types can be set. Element
types are determined by geometry. Vertical line elements are considered to be
columns, horizontal ones are handled as beams, horizontal domains as floors,
vertical domains as walls.

Opaque Transparent

User’s Manual 43

2.15.7. Guidelines

Helps in editing the geometry of the model. Guidelines can be defined in the
global coordinate system. This way an arbitrary grid can be created,
intersections can be determined and distances can be set. The cursor identifies
the guidelines. See... 4.7 Editing Tools

$
The guidelines are displayed as blue
dashed lines. The display of the
guidelines can be enabled or disabled
in the Display Options menu (or icon)
in the Switches section.

Places a vertical guideline at the current position of the cursor.

Places a horizontal guideline at the current position of the cursor.

Places a vertical and a horizontal guideline at the current position of the
cursor.

Places an oblique guideline at the current position of the cursor.

Places a pair of orthogonal oblique guidelines at the current position of the
cursor.

In perspective view all the guidelines are displayed but only oblique guidelines
can be placed.
You can change the position of a guideline with the mouse by dragging it to a
new position. You can remove (delete) a guideline by dragging it off the
graphics area.

Guidelines can be entered numerically by coordinates. Clicking with
the mouse on a guideline or selecting Settings/Guidelines Setup command from
the main menu, the following dialog is displayed:

a
b

a: is the angle of the guideline’s projection on the X-Y plane and the X axis.

b: is the angle of the guideline and its projection on the X-Y plane.
guideline
44 AxisVM 8+Release 4

2.15.8. Geometry Tools

The icons of Geometry Tools allow you to lock the direction of drawing a line.

Perpendicular Parallel

Begin to draw a line. Click the Perpendicular or Parallel icon then click an
existing line or click two points to define the direction. The cursor will move
perpendicular or parallel to this baseline.

Perpendicular to a plane

Begin to draw a line. Click the Perpendicular to a plane icon then click the
domain defining the plane. The cursor will move perpendicular to the plane.
The plane can also be defined by clicking three points.

These icons can be conveniently used while editing the geometry of the model
or defining section planes.

Line towards a midpoint

Using of icon: begin to draw a line then click startpont and endpoint of
another line. Midpoint will determine the direction.

Bisector

Using of icon: begin to draw a line then click the two legs of an angle. Bisector
will determine the direction of the line.

2.15.9. Dimensions Lines, Symbols and Labels

This group of functions lets you assign associative orthogonal and aligned
dimension lines or strings of dimension lines to the three dimensional model,
as well as angle, arc length, arc radius, level and elevation marks, labels
or result values. Click on the Dimensions icon to display the Dimension
Toolbar. That will allow you to select the proper dimension tool. Click on the
left-bottom icon of the Dimension Toolbar to set the parameters of the selected
tool.

You can change the position of dimension lines or labels at any time
by dragging them to their new position. If the dimension lines were associated
with the model their position and dimension will be continuously updated
as you modify the geometry of the model.

Baseline
Baseline
User’s Manual 45

2.15.9.1. Orthogonal Dimension Lines

Associative orthogonal dimension lines or strings of dimension lines, parallel
with the global X, Y, or Z axes can be assigned to the model by following the
next steps:
1. Click on dimension line start point and on the end point. If these points
are connected by a line you can just click on the line.

2. Move the mouse. The position of the dimension line depends on the
direction in which you moved the mouse. There is one exception: when
the segment is not parallel with any global plane and the editing is in
the perspective view. In this case you have to select the direction
dX, dY, or dZ from the toolbar.
3. Click the left mouse button to set the final position of the dimension
line.
To insert a string of dimension lines, click on the points in the corresponding
order or on the lines if any. Steps 2 and 3 are the same as for the individual
dimension lines. A string of dimension lines can be selected at once if you click
on one of them while depressing the Shift key. It allows you to move it as
a group. To change the position of a group segment individually select it using
the selection rectangle and drag it to its new position. As a result this
dimension line will be removed from the group (it can be moved individually).

Smart dimension
lines
A string of dimension lines can also be created by turning on the smart
dimension lines. If you enable this function by pressing the button, you have
to select only the end points of the string, assuming that the intermediate
points were not generated by a domain mesh command. All intermediate
dimension lines will be created automatically.

An example of smart dimension lines
If the dimension line is assigned to the points of a model, it will always behave
in an associative way (e.g. will move with the model when the model is
changed or resized or moved).

Orthogonal and Aligned Dimension Line Settings

46 AxisVM 8+Release 4

Tick mark

Lets you set the tick marks of the dimension lines. You can select from nine
predefined symbols.

Color

Lets you set the color of dimension lines individually. You can get the color
from the active layer. The dimension lines, marks, and texts are placed on the
Dimensions layer by default but you can change it any time.

Sizes Lets you set the drawing parameters of the dimension line.

Dimension style/
Extension style

Lets you to set the type and thickness of a dimension or extension line.
You can choose a predefined value or get it from the active layer. You can turn
on/off the display of extension lines.

Label orientation

Lets you set the orientation of the text labels of the dimension lines (Always
horizontal, Always vertical, Auto horizontal/vertical, or Aligned to dimension
line) inside or outside the dimension line.

Use defaults Lets you restore the default setting.

Apply font to all
symbols
Apply the same font to every dimension line.

Save as default
setting
Lets you save the current setting as default setting.

Apply to all
dimension lines
Applies the current setting to all existing orthogonal or aligned dimension lines
to ensure a uniform look.

Layers

Lets you select/define/set layers where the dimension lines will be placed.
If there are no layers defined when you start defining dimension lines,
a Dimension layer will be automatically created.
See... 3.3.3 Layer Manager

Text Parameters

Allows to you to define the settings of the text on the dimension lines.

Measured value Allows you to place the measured value on the dimension line, using the
current prefix and suffix settings. By clicking the Units and formats button the
number format can be set in the Dimensions section of the Settings / Units and
Formats dialog box.

Display unit of
measurement
Display of the unit of measured value.

Units and Formats.. To change the current font parameters click the button below the Units and
formats... button.

User’s Manual 47

Prefix

Sets the prefix used with the text on the dimension lines. You can choose
from the following options:
Auto (dX, dY, dZ, dL = [depending on the direction])
Auto (DX, DY, DZ, DL = [depending on the direction])
User defined (this option will require you to enter the prefix).

Suffix Sets the suffix used with the text on the dimension lines.

2.15.9.2. Aligned Dimension Lines

Assigns aligned dimension lines or a string of dimension lines to the model.

The steps are the same as the steps of creating an orthogonal dimension line
(see... 2.15.9.2 Aligned Dimension Lines).
The plane of the parallel dimension line is determined automatically. There is
one exception: when the segment is not parallel with any global plane and the
editing is in the perspective view. In this case you have to select the direction
X, Y, or Z from the toolbar. The plane of the section line will be defined by the
segment and the selected global axis.

Associative angle dimensions, as the symbol of the angle between two
segments, can be assigned to the model in the following steps:
1. Click on start point and on the end point of the first segment.
If the points are connected by a line you can just click on the line.

2. Click on start point and on the end point of the second segment.
If the points are connected by a line you can just click on the line.

3. Move the mouse. The position and
radius of the angle dimension will be
determined by the mouse movement.
Based on the position of the mouse,
the angle, supplementary angle
or complementary angle dimension
can be entered.

4. Click the left mouse button to set the
angle dimension in its final position.
plane of dimension line based on X-axis

plane of dimension line based on Y-axis

plane of dimension line based on Z-axis
48 AxisVM 8+Release 4

By clicking the Units and formats button the angle number format can be set in
the Dimensions section of the Settings / Units and Formats dialog box.

2.15.9.4. Arc Length

Creates arc length dimension symbols in your model.
To assign this symbol to a full circle click any point of the circle and drag the
symbol.

To assign this symbol to an arc click any point of the arc and drag the symbol.
To assign this symbol to a part of an arc click any endpoint of the arc, click the
middle point of the arc and drag the symbol.

2.15.9.5. Arc Radius

Creates arc radius dimension symbols in your model.
To assign this symbol to an arc click any point of the arc drag the symbol.

User’s Manual 49

2.15.9.6. Level and Elevation Marks

Creates associative level and elevation marks in your model.
By clicking the Units and formats button the number format can be set as the
unit of Distance in the Geometry section of the Settings / Units and Formats
dialog box. This is the unit and format used in the Coordinate Window.
See...3.3.6 Units and Formats

Level marks can be placed in top view, by clicking on the desired point.
The top view is defined as the view in the direction of gravity (You can
change it in the Settings / Gravitation dialog).
See... 3.3.7 Gravitation

Elevation marks can be placed in front view, side view, or in perspective,
by following the next steps:

1. Click on the point you want to
mark.

2. Move the mouse in the direction
you want to place the elevation
mark, and click to set the symbol
in its final position.

Sets the level and elevation mark parameters.

Level Selects the level mark symbol, and sets its size and format.

Elevation Selects the elevation mark symbol, and sets its size and format.

50 AxisVM 8+Release 4

2.15.9.7. Text Box

Creates an associative text
box in your model.
You can enter multiline
text in a text box. The text
will use the same text
formatting within a text
box.

You can create a text box
in the following steps:

1. Enter the text in the Text box parameters window, or in case of a single line
text enter it directly into the edit field of the Toolbar.

2. Click on the point to which you want to assign the text box.

3. Move the mouse to the desired position and click to set the text box
in its final position.

Color

Sets the color of the text, frame, and extension line. You can get the color from
the layer.

Text box

These switches set the drawing parameters of the text box, frame, and
extension line, the transparency and alignment of the text, and the d distance
of the extension line from the reference point (to which the text box is
assigned to).

Font Sets the text font, style and size.

You can reload and change default settings, apply text box or font parameters
to all existing text boxes

User’s Manual 51

Active Links Active links can be placed in text boxes to attach any external information tot
the model. If the text contains a file reference or a link to a web page clicking
the text box launches the application associated to the file or URL instead of
opening the above dialog. To change the text select text box first
(e.g. Shift+click) then click into the box.

File reference A file reference is made of the -> characters and a file name. E. g.:
->C:\MyModel\Reports\Details.doc
If no full path is specified AxisVM starts from the folder of the model. So if our
model is in C:\MyModel we can enter: -> \Reports\Details.doc
Clicking the text box starts the application associated to the file type. This way
we can attach pictures, movies, sounds, Excel tables or other documents to any
part of the model.

URL Supported protocols and link formats are: http://..., ftp://..., https://..., file://...,
www. ... Clicking the text box the default web browser launches and opens the
web site or file. If the text contains more than one URL, the first one is used.

2.15.9.8. Object Info and Result Text Boxes
Object info text box

Element or load properties appear in the text box depending on the current tab
(Geometry, Element or Loads). Information text box parameters can be set in
a dialog:

Result labels

When displaying results the cursor determines the value of the current result
component on nodes, mid-side nodes, surface centers, or intermediate points
of beams or ribs and shows it as a tooltip. The text of the tooltip is automati-
cally entered in a text box.
The steps of result labeling are similar to creating a text box.
The result text box is visible only when the selected result component is the
same as the one that was selected when the result text box was created.
For example an My result text box is displayed only when the My component
is selected as the current result component.

52 AxisVM 8+Release 4

Result text box options can be set in a dialog box:

In this load case only
Result label is visible only in the load case in which it was created.
In all load cases
Result label remains visible regardless the load case. The actual values will
be updated on changing the case.
For this result component only
Result label is visible only if its result component is displayed.
For all result components
Result label remains visible regardless the displayed result component.

Result label text options :

Element: Include element type and number.
Component: Include result component name.
Case: Include name of the load case, combination
or description of the critical combination.
Unit: Include unit name.
User’s Manual 53

Below the button of Use defaults three checkboxes helps to customize the text
box:

Apply font to all text box
After clicking the OK button only the font of all text boxes will change.
Save as default setting
New text boxes will appear using the current settings as default.
Apply parameters to all text box
After clicking the OK button parameters of all text boxes will be set to these
values.

Layer Manager

[F11]
Lets you create new layers or modify existing ones.
This function is also available from the menu as Settings\Layer Manager.
See... 3.3.3 Layer Manager

2.15.9.9. Isoline labels

Lets you place a series of labels to isolines.
1. Click to the Isoline labels icon
2. Enter two points defining a line segment
3. The labels are placed at the intersections of the segment and the isolines

54 AxisVM 8+Release 4

2.15.10. Parts

Lets you create sets of structural elements called parts. Working with parts
makes the pre- and postprocessing easier.
AxisVM allows you to display one or more parts, called active parts, at the
same time. In addition, if the Parts check box is enabled the commands will
only affect or refer to the entities of the active parts. The name of the current
part is displayed in the Info window. If more than one part is turned
on n parts is displayed, where n is the number of active parts.

You can activate an existing part by clicking its name in the list box.
Parts can also be activated without opening this dialog box by simply clicking
the Parts speed button (at the bottom of the screen).

New Creates a new part (a set of model entities).
You must assign a name to each new part. You must then define the new part
by selecting entities (using the Selection Icon Bar if necessary) in the active
display window.
Modify Lets you modify the selected part. When the selection menu appears,
the entities of the model that are in the part are displayed as selected.
Delete Lets you delete the selected part from the list. This command will not affect
the model.
Delete All Lets you delete the definition of all the parts. No part of the model is deleted.

Logical Set
Operations
Creates a new part by performing
logical set operations on the parts
of a model. You have to specify
the set operations. To enter the
name of a part, double click on
the respective name in the list.
Use the % symbol to include the
entire model. For example: %-
Columns will create the part that
will include the entire model less
the part named Column.
Clicking on the Create button,
you can enter in the Name field
the name of the newly created
part.

If you want to use the +, -, , (, ) characters in the name of a new part, you need
to put the name between “” marks (example: "floor +12.00").

User’s Manual 55

Display switches Display switches work in the following way:
All
Turns on or off all the parts in the list.
Parts
If it is on only the parts checked in the list are displayed. If it is off the
entire model is displayed.
F

When working on parts, only the data of the active parts will appear in the
tables by default.
Auto Refresh
If it is on turning on or off parts will immediately cause a redraw. If it is off
the screen is updated only after clicking the OK button.
Refresh all
If it is on parts will be turned or on off in all window panes in multi-
window mode. If it is off part settings will be updated only in the active
panel.
Show non-visible parts grayed
If it is on the entire modell wireframe is also displayed in gray to help
identification of model parts.

2.15.11. Sections

Lets you create section lines and planes through any surface model, that can be
used to process the results (displacements, internal forces, etc).
If a truss, rib or beam is within an active section plane and the result
component has values on these elements a diagram is displayed on these line
elements too.

56 AxisVM 8+Release 4

The dialog works similar to the Parts dialog.
Section lines, planes and segments can also be turned on and off using a speed
button at the bottom toolbar.
If the result display mode is Section result diagrams are displayed only on
section lines, planes and segments.
To reduce the complexity of drawings display of individual sections lines,
planes or segments can be controlled to appear only in a certain load case
and/or for a certain result component.

New section
segment
To define the segment enter two points of a domain or on domains in the same
plane.
Setting the radio buttons you can control how the internal forces diagram will
be displayed. Left or right segment width can also be specified.
Diagrams are usually displayed perpendicular to the element plane but check-
ing the option Draw diagram in the plane of the elements rotates the diagram into
the plane. In the Display Parameters dialog this parameter can be turned on/off
for all section segments.

Display of the resultant integrated values

Display of the average values

New section plane Click New section plane and assign a name to the section. This type of section is
based on a plane. Click or enter two points to set the section plane. Then click
OK in the Selection Icon Bar to save. In perspective view you have to click
or enter three points to set the section plane.
Section planes are displayed as rectangles of dotted lines. You can
enable/disable the display of section plane rectangles.

Section planes are useful when
you want to display results only
along a certain line through the
entire structure.

User’s Manual 57

New section line Click New section line and
assign a name to the section.
You then have to select sur-
face edges or beam elements
that define the section line.
Then click OK in the Selection
Icon Bar to save. Section lines
can be discontinuous.

The checked section lines, planes and segments are active.
You can use Auto Refresh and Refresh All checkboxes, New, Modify and
Delete buttons the same way as in the Parts dialog.

F
The tracelines of the section lines are not correlated with the directions of the
result components displayed.

2.15.12. Find

Finds the entity having a specified index, and moves the cursor over it.
If Select element is turned on the element found will also be selected (displayed
in purple).

2.15.13. Display Options

58 AxisVM 8+Release 4

Auto Refresh: If enabled, any setting change will result in an automatic refresh
of the active graphics window display.
Refresh All: If enabled, the changes will affect the settings of all graphics
windows.

Symbols Enables/disables the display of the symbols.

Graphics Symbols Mesh
Enables the display of the inner mesh lines.

$
When disabled only the outlines are displayed.
Node
Enables the display of the nodes (small black rectangles).
Surface center
Enables the display of the center point (selection point) of the surface
elements.

$
Node-to-node link el ements are displayed as solid green lines with an
arrowhead showing the location of the link.
Line-to-line link elements are displayed as solid green lines with an
arrowhead showing the location of the link and dashed green lines
at the line endpoints.
Reference
Enables the display of the references.

$
Red vector, crosshairs or triangle.
Cross-section shape
Enables the display of the shape of the cross-section of the truss/beam/rib
elements.

$
The user-defined cross-sections will be displayed as rectangles that
circumscribe the shape of the cross-sections.
End releases
Enables the display of the end release and edge hinges.
End release:

Auto Refresh If it is turned on any change in settings will make the active panel redrawn
immediately.

Refresh All Changes will affect all panels in multi-window mode.

60 AxisVM 8+Release 4

Labels

Numbering

Displaying the number of nodes,
elements, materials, cross-sections,
references.
For meshed line elements checking
Use finite element numbers displays the
number of finite elements instead.

Properties Enables the display of the name and values of materials properties, cross-
sections, element lengths or thicknesses, load values, masses.
If the Units option check-box is enabled, the labels will include the units as
well.

Display The display of the actual parts and guidelines can be turned on and off.

Parts
Enables/disables the display of parts.

Guidelines
Enables/disables the display of the guidelines.

2.15.14. Options

Allows the selection of the options for the settings of the grid, cursor, editing,
drawing parameters, and design code.

2.15.14.1. Grid and Cursor
Grid

The grid consists of a regular
mesh of points or lines and
helps you position the cursor
to provide a visual reference.
Depending on its type the grid
is displayed as:
Dot grid – axes are displayed
with yellow crosses , points in
gray
Grid lines – axes are dis-
played in yellow, lines in gray.

You can set the grid parameters as follows:
Display
Displays the grid if the check-box is enabled.

∆X, ∆Y, ∆Z
Sets the spacing of the dots/lines of the grid in the direction X, Y or Z.

You can set the cursor step parameters as follows:
Mouse Grid
Restricts the movement of the mouse cursor to an invisible grid specified
by the cursor step values below.

∆X, ∆Y, ∆Z
Restricts the cursor movement to regular intervals. Each time you press a
cursor movement key the cursor moves in the corresponding direction
(X, Y or Z) one step (∆X, ∆Y or ∆Z respectively).

Ctrl x
Sets the value of a factor that increases or decreases the cursor step size
if you press the [Ctrl] key when you move the cursor. This allows you to
achieve adequate positioning accuracy.
F
The cursor step is ignored if you position the cursor on a line. In such a case,
the cursor will move along the line.
When using with constraints, the cursor step is applied in the constrained
direction with the DX value.
See... 4.7.4 Constrained Cursor Movements
F
If the grid step and the cursor step is set to the same value, nodes will be placed
snapped to the grid.

62 AxisVM 8+Release 4

2.15.14.2. Editing
Constraint Angle During the model editing the
movement of the cursor can
be constrained.
Using the [Shift] key while
moving the cursor, the
movement direction can be
set. In this case the
constrained movement of the
cursor will be based on two
types of angles (for other type
of constrained movements
see...4.7.4 Constrained Cursor
Movements).

Auto Sets commands that are applied automatically if the corresponding check-box
is enabled.
Intersect :
Sets the line intersection handling. At intersection points of lines a node will
be generated and lines will be bisected. If surfaces are intersected by lines,
they will be split, and the resulting elements will have the same material and
cross-sectional properties as the original.
Part management :
Any entity drawn or modified after the check-box is enabled will be
associated with all of the active parts.
Refresh :
Sets the display refresh mode to automatic.

Editing Tolerance If two nodes are closer than the value set as the editing tolerance, they will be
merged in the case of a mesh check. This value is also used when comparing
surface thickness or beam length.

Cursor
identification

The element under the cursor is identified if it is
within an adjustable cursor identification
distance. The unit for cursor identification
distance is pixels.

If more than one element is within this range the closest one will be identified.
See... 4.7.1 Cursor Identification

Plane tolerance Nodes of domains and surfaces must be in plane. If a node of a domain
or surface deviates from this plane more than the given value the element will
be deleted. Plane tolerance can be specified in two ways:

Relative [‰] per thousand of the biggest extension of the
element polygon
Absolute [m] a given value

2.15.14.3. Drawing
Load symbol display
factors
Sets the display size of the load
symbols. This factor is applied
when the checkbox in the Sym-
bols icon / Graphics Symbols /
Load is enabled. These values do
not affect load values.
Force
Sets the display size of the
symbol of concentrated force
loads.
Moment
Sets the display size of the
symbol of concentrated moment
loads.
Line / surface load
Sets the display size of the symbol of line / surface loads.

Contour line angle Sets the display of the inner mesh lines (between adjacent surface elements).
The common edge of two or more surface elements is displayed if the angle
enclosed by the normal to the planes of the elements is larger than the value
set here.

Zoom factor Sets the scale of magnification/reduction of the zoom commands associated to
the [+] and [-] keys.

2.15.15. Model Info

Shows the main parameters of the
model.

Displayed
edge
Edge not dis-
played
64 AxisVM 8+Release 4

2.16. Speed Buttons
The quick switches toolbar allows you to change the display settings without
entering the Display Option/Symbols or Options dialog. The icons are located
in the bottom right corner of the graphics area.

Auto Intersection

Mouse Snap

Parts

Display Parts of the selected elements

Workplanes

Section Lines & Planes & Segment

Display Mesh

Display Loads Symbols

Display Symbols

Display Local Systems

Numbering

Background Layer

Background Layer Detection

F
Some of these settings are available also from Display and Service icons.

2.17. Information Windows
The information windows are situated in the graphics area. You can move
these windows on the screen by clicking title bar, holding down the left mouse
button, and dragging it to a new location on the screen.

2.17.1. Info Window

Shows information about the display of the results such as:
active part(s), current perspective setting, type of analysis,
current design code, current load case or load combination,
solution errors, current result component.
For the explanation of E(U), E(P), E(W), E(EQ) parameters
see Analysis and Static Analysis.

2.17.2. Coordinate Window

See... 4.4 Coordinate Window
User’s Manual 65

2.17.3. Color Legend Window
Displays the color legend corresponding to the result component being
displayed in the postprocessor. You can resize the window and change the
number of levels simply by dragging the handle beside the level number edit
box or entering a new value. Colors will be updated immediately.
You can set the color legend details in the color legend setup dialog box.
To open this dialog box simply click the color legend window.

Color Legend
setup

Limits Setting criteria for the interval limits:
Min/max of model
Sets the lower and upper limit values to the minimum and maximum
values of the entire model. Intermediate values are interpolated.
Min/max of parts
Sets the lower and upper limit values to the minimum and maximum
values of the active parts. Intermediate values are interpolated.
Abs. max of model
Sets the lower and upper limit values to the maximum•absolute value of
the entire model with the respective negative and positive signs.
The intermediate values are interpolated.
Abs. max of parts
Sets the lower and upper limit values to the maximum•absolute value of
the active parts with the respective positive and negative signs.
The intermediate values are interpolated.

Custom
Click an item of the list on the left to edit its value. If you are in editing
mode you can navigate through the list by UP and DOWN keys and edit
the current item. When you click OK the series of interval values must be
monotonically decreasing from top to bottom.
Auto Interpolate
If Auto Interpolate is checked the series will be recalculated each time you
enter a new value. If you enter a new top or bottom value the recalculated
series will be linear between top and bottom values. If you enter a new
value at a middle interval the recalculated series will be bilinear, i.e. linear
between the top and the new value and between the new and the bottom
value but steps may differ.
By step value
Color values are determined by the given step ∆. When entering a new
level value the other levels will be recalculated using the step. Switching
from other crieria the array starts from the lowest value and using the
latest step value.
66 AxisVM 8+Release 4

You can save the settings of the scale using the Save As button. To review
saved settings click the ... button.
Standard interval limit settings are also available directly from the color legend
window popup menu. To activate popup menu click right mouse button on
the window.

Calculate
When displaying reinforcement values click
Custom and Calculate to get the amount of
reinforcement from rebar diameters and
distances for the selected list item.
F
When displaying actual reinforcement schemes
AxisVM does not assign color to numerical
values but to different rebar configurations.
It can be set to display all schemes or just
those within the active (visible) parts.

2.17.4. Perspective Window Tool

See... 2.15.3 Views

User’s Manual 67

3. The Main Menu
3.1. File

The menu commands are described below.

3.1.1. New Model

Creates a new untitled model. Use this command to start a new modeling
session. If you have not saved the current model, a prompt appears asking
if you want to save it first. Refer to the Save and Save As commands for more
information on how to save your current model.
You must specify a name for the new model. You can select the appropriate
Standard and system of units. You can enter specific information in
the Heading section, that will appear on each printed page.
A new model uses the default program settings.

68 AxisVM 8+Release 4

3.1.2. Open
[Ctrl]+ [O]
Loads an existing model into AxisVM. If you have not saved the current
model, a prompt appears asking if you want to save it first. Refer to the Save
and Save As commands for more information on how to save your current
model.
Selecting this command will bring up the Open dialog box.
If the folder name appearing in the dialog box is what you want, simply enter
the file name in the edit box or select it from the list box. If the directory is not
what you want, select the drive and directory names along with the file name.

F
AxisVM saves your model data in file names appearing as Modelname.AXS
(input data), and Modelname.AXE (the results). Both file contains the same
identifier unique for each save which makes it possible to check if AXS and AXE
files belong to the same version of the model.

3.1.3. Save
[Ctrl]+ [S]

Saves the model under the name displayed at the top of the AxisVM screen.
If you have not saved the model yet, the Save As dialog box automatically
appears prompting you to enter a name. Use the Save As command if you are
changing an existing model, but want to keep the original version.

3.1.4. Save As
Names and saves the model. Use this menu command to name and save a
model if you have not saved the model yet, or if you are changing an existing
model, but want to keep the original version.
Selecting this menu command will bring up the Save As dialog box.

Converting models

Models created with previous AxisVM versions (if applicable) will be
converted into the current version file format when you open them for the first
time.
F
The File / Save As / File Format command lets you save the model in Axis
version 5.0 / 6.0 / 7.0 formats.

DXF file Saves the geometry of the model to a DXF file format for use in other CAD
programs. The geometry is saved with actual dimensions, in a
Modelname.DXF file.
Selecting this menu command will bring up the Export DXF dialog box,
that lets you specify the units of measurement in the exported file.
Three different formats are available for DXF output.
- AutoCAD 2000 DXF file
- AutoCAD R12 DXF file
- AutoCAD reinforcement design file

F
ArchiCAD can read the aof file only if the Axisvm.apx file is present in its
AddOns folder.

Xsteel file Two different file formats are available:
XSteel ascii file (*.asc)
Saves the geometry of the model into a file format that is recognized by the
Xsteel software. The file includes the coordinates of i and j-end nodes, the
cross-sectional properties and the reference point of truss and beam
elements.
DSTV file (*.stp)
Saves the data of the truss and beam elements (endpoints, material, cross
section, reference) as a standard DSTV file. This file format is supported by
several steel designer CAD software.

Bocad file Saves the geometry of the model into a file format that is recognized by the
Bocad software. The file includes the coordinates of i and j-end nodes, the
cross-sectional properties and the reference point of truss and beam elements.

StatikPlan file For StatikPlan AxisVM exports a DXF file including the contour of the
reinforced concrete plate, the calculated reinforcements as isolines and the
result legends on different layers.

PianoCA file Generates a *.pia interface file for PianoCA. It includes the data, supports,
loads and the calculated results of the selected beam elements.

CADWork file Creates a DXF file to use in CADWork reinforcement detailing software.
Only selected domains will be exported.
As CADWork works in 2D, selected domains must be in the same plane.
Each domain in the DXF file is transformed to a local X-Y coordinate system,
Z coordinate represents the calculated amount of reinforcement.

Export Selected
Only
Exports only the elements that are in the current selection set.

Coordinate units The coordinate units of the exported file can be selected here.
The default unit is meter [m].

70 AxisVM 8+Release 4

3.1.6. Import

ArchiCAD *.ach Imports an object-oriented mesh from an ACH file into AxisVM. The ACH file
format was developed by Inter-CAD Kft. specifically for Graphisoft ArchiCAD
software, in order to allow integrated design of complex structures
architecturally designed with ArchiCAD and numerically analyzed with
AxisVM.

If you have an existing ArchiCAD model the new model always overwrites it.
AxisVM generates the cross-sections from the geometric data of the
corresponding ArchiCAD objects.
See... 4.9.18 Creating model framework from an architectural model

F
In order to be able to export an ACH file from an ArchiCAD project, you have to
make sure that the Axisvm.apx file is copied from your AxisVM setup CD to the
ArchiCAD 6.0 (or later version) AddOns folder.

To save an ArchiCAD model as ACH file you must follow within ArchiCAD
the steps below:
1. Open the ArchiCAD model file
2. Enable the display of the levels and objects that you want to be
included in the analysis
3. Select a perspective display of the model
4. Apply the Save As command (File menu)
5. Select the AxisVM file format option
6. Enter a filename (the file will be saved as filename.ach) and specify the
folder where you want to save the file
7. Close the Save As dialog with the OK button.

AutoCAD *.dxf

Imports a geometry mesh from a DXF file (drawing interchange file) exported
in AutoCAD 12, 13, 14 and 2000 format into AxisVM. The layers of the
imported file are loaded into the Layer Manager (see...3.3.3 Layer Manager).
If the file date of the imported file has changed, the Layer Manager will ask
if you want to update the layers.
Selecting this menu command will bring up the Import DXF dialog box.
F
The ellipses will be converted to polygons only if you load them as active mesh
otherwise they remain ellipses.
Import Model

User’s Manual 71

Parameters Input units
You need to specify the length unit used in the imported DXF file.

Maximum deviation from the arc [m]:
Importing a DXF file as an active mesh, ellipses will be converted to poly-
gons based on this value.

Geometry check tolerance
When you import a DXF file as an active mesh, AxisVM checks for coin-
ciding points (nodes) and lines in your model, and merges them.
You can specify the maximum distance to merge points. Points that are
closer together than the specified distance are considered to be coinciding.
The coordinates of the merged points (nodes) are averaged.
You must always set this to a small number relative to your model dimen-
sions.

Import As You must specify whether you wish to use the imported DXF file as an active
mesh or as a background layer.

Active mesh (nodes&lines)
The imported geometry is considered as if it were created with AxisVM
commands.

Background layer
The imported geometry is used as a background layer that is displayed but is
inactive as a mesh. Import a DXF file as background layer when you want to
create the model based on architectural plans or sections. You can use the
entities in the background layer as a reference during editing your model.

Import Mode You can choose between overwriting the former geometry or adding a new
geometry to the former one

Place

Lets you specify the plane of the DXF layer (X-Y, X-Z, or Y-Z).
The Place button allows to graphically position the imported DXF drawing in
your model space.

IFC 2.0, 2x and
2x2, 2x3 *.ifc file
Imports objects from an architectural model saved as an IFC file. Imported
objects can be displayed as a 3D background layer or can be converted to a
native model by assigning materials, cross-sections etc. to them. Existing
architectural models are always overwritten by the new one.
You can import object based architectural models from ArchiCAD, AutoDesk
Architectural Desktop, Revit Structure, Revit Building Nemetscheck Allplan,
Bocad and Xsteel. Programs.
If the AxisVM model already contains an architectural model it can be over-
written or updated in the import process.
See... 4.9.18 Creating model framework from an architectural model

F
When exporting a model from ADT (Architectural Desktop) turn off the auto-
matic intersection of walls before creating the IFC file.

72 AxisVM 8+Release 4

AxisVM *.axs Imports a model from an existing AxisVM file into AxisVM, and merges it with
the current model.
During the merging process, the Geometry Check (See... Section 4.8.11)
command is automatically applied. If there are different properties assigned to
the same merged elements, the properties of the current model will be
retained. Load groups and combinations if any, are appended to the existing
ones as new groups and combinations, and the load cases as new cases.
If no load groups or combinations are defined in the imported model, the load
cases will be appended to the existing ones as new cases. If the same case exists
in both models, the loads will be merged.

If both models contains loads that are limited to one occurrence (e.g. thermal)
in the same load case, the load in the current model will be retained.
The Section Lines/Planes Parts with the same name are merged, otherwise
they are appended.

When importing an AxisVM file the following dialog is displayed:

Use the Place button to graphically position the imported model in your
model’s space.

Stereo Lithography
*.stl file
Reads the triangular mesh describing the surface of a model from a file in STL
format. Multiple nodes and degeneated triangles are filtered out.

3.1.6.1. Tekla Structure – AxisVM connection
Setup The connection between the two software is made through a COM server en-
abled to run AxisVM. To make the connection work first the COM server must
be registered within the operating system (in the Registry) then Tekla Struc-
tures must be notified that a compatible server is available.
AxisVM setup automatically performs these registering operations, however
if Tekla Structures is not installed the second registration cannot be completed.
Therefore after installing Tekla Structures the registration has to be started
again by running two batch files from the AxisVM program folder
!REGISTER_AXISVM.BAT
!REGISTER_TEKLA.BAT
If connections fails any time it is recommended to run this registration again.

Connection After a successful registration the model built in Tekla Structures can be trans-
ferred to AxisVM in the following way: click Analysis & Design models... in the
Analysis menu then click the Properties button to set AxisVM AD Engine as the
Analysis engine.

User’s Manual 73

If AxisVM AD Engine does not appear in the dropdown list the registration
was not successful and has to be repeated.

Getting back to the Analysis & Design models dialog click Run to start the trans-
fer of the model. The process status is displayed in dialog. If the transfer is
completed successfully click the OK button to see the model in AxisVM.

74 AxisVM 8+Release 4

The model transferred to AxisVM:

Loads and load cases specified in Tekla Structures are also converted.

3.1.7. Page Header
Lets you specify a header text (two lines), which contains the name of the
project and designer. It will appear on the top of every printed page.

User’s Manual 75

3.1.8. Print Setup

Allows setting the parameters of the default printer.
This is a standard Windows dialog therefore its language corresponds with the
language of the installed operating system.

3.1.9. Print
[Ctrl]+ [P]
Lets you print the model according to the current display settings. Allows the
setup of the printer, and of the page.

Printing drawing

Send To
Lets you send the output directly to the printer/plotter or to a graphics file
(DXF, BMP or Windows Metafile [WMF/EMF]).
Printer
Lets you select and setup the printer.
If a file is selected as output, the printing will be stored in the Name.prn
file, where Name is a file name to be entered. You can set the number of
copies required. The Setup button invokes the standard Windows Printer
Setup dialog where you can change printer and printer settings in detail.
Scale
Lets you set the scale of the drawing to print. In case of perspective or
rendered view or if the output is sent to a Windows Metafile the scale
cannot be set.
Margins (Printer/DXF)
Lets you set the size and the units of the page margins. You can also drag
margin lines within the preview area by their corner and midside handles.
Bitmap Size (BMP, JPG)
Lets you set the bitmap size in pixels, inch, mm or cm and bitmap
resolution in dpi (dots per inch).
Preview
Lets you view the printed image prior printing. If you select Printer as a
target the graphics cursor turns to a hand whenever it enters the preview
area. By pressing the left mouse button and moving the mouse you can
specify an additional panning which will affect the printed output only.

Current printer Printer setup Output
76 AxisVM 8+Release 4

Page Header
Lets you set the date and remark that will appear on each page, and the
starting number for the page numbering.
Orientation
Lets you set the orientation of the page.
Color Options
Lets you select printing in grayscale, color, or black and white.
If your printer cannot print in color you may get different results in the
first two cases. If you select Grayscale the output will be converted
to grayscale using an internal grayscale palette of AxisVM. If you select
Colors the conversion to grayscale will be performed by the Windows
printer driver. Try both to find which works better for you. When black
and white printing is selected, all entities are printed in black.
Paper size
Lets you set the size of the paper.
Change Fonts
Lets you select fonts to be used in printing and set the font size.
Pen widths
Sets the size of the pens for printing.
Thick lines are used for drawing
supports and rigid elements. Medium
lines are used for isolines and section
line. Thin lines are used for elements
and geometry and other entities.

Windows to Print
Lets you print either the active window or all windows displayed.

Printing to file When Print to File is selected the printing is redirected to a file, name.prn that
you can print anytime later.

If the file name.prn already exists, you can add your printing to it, or overwrite
it.

If you want to print only into files, you can set the operating system to do so in
the Start/Settings/Printers choosing Properties and setting the Print to the Port
as File. In this case you can not append print files.

User’s Manual 77

Printing table When printing from the table browser, you can set the pages (all/even/odd)
of all/current/selected pages you want to print.

3.1.10. Printing from File
You can print the prn file you created from the following window.

You can print more than one prn file at a time. You can set the printing order
with the up/down arrows in the right of the file list box, or dragging the file
names to a new position with the mouse.

78 AxisVM 8+Release 4

3.1.11. Model Library

The File/Model Library command lets you preview, get information and manage
your model files.
As in Open and Save As dialog windows the standard file access dialog box
items are displayed, but in the list box you can select multiple files.

$
The AxisVM model files are marked with the symbol. If a model has a result
file the symbol has a blue right-bottom corner, .

New
Creates a new sub-folder in the current folder with the name you enter.

Copy
Copies the selected files to a different folder. You can specify whether to
copy the result files or not.

Rename/Move
Renames the selected files in the current folders or moves them into a
different folder.

Delete
Deletes the selected files from the current folders. You can specify to
delete only the result files or all.

Open
Opens the selected file for editing.

$
AxisVM files are marked with . If a result file is available, the bottom right
corner of the icon is blue.

Preview
Shows the model wireframe in front, side, top view or in perspective
depending on the model dimensions. Model information is also displayed
in a list.

Close
Quits the Model Library.

Current model preview
Current folder Current drive
User’s Manual 79

3.1.12. Material Library

AxisVM provides a preloaded material library (that contains the most
frequently used structural materials) and allows you to create material
property sets that you can use over and over again in many different models.
You must assign different names to each material property set.

The material library window can also be opened using the Table Browser icon
and by selecting Libraries/Material Library. (see... 4.9.6 Line Elements,
4.9.18 Creating model framework from an architectural model).
See the detailed description of the Table Browser in section 2.9.

Properties of
materials
This table contains the properties of materials often used in civil engineering to
the MSz, Eurocode, DIN-1045, DIN-1045-1, NEN, SIA-162, a STAS and Italian
codes. You can add, modify, or delete existing material data. In case of entering
a new material with an existing name it will be added as
materialname_number. These materials can be used in any model.

F
Changes in the material library does not reflect in models using the modified
material.
When entering a new material, the following dialog is displayed:

Define new
material
[Ctrl+Ins],
Change
material properties

Definig new material or clicking to a
non-editable column (eg. national
design code, type) a dialog appears,
in which all material properties,
calculation and design parameters
can be defined or changed. The fields
containing the basic properties in-
dependent of the design code can be
edited in the table.
When a material with a name
identical to one existing is entered an
index is attached to the name
(name_index) to differentiate from the
existing one.

In case of timber materials:
ρ is the air dry mass density (12% humidity) and, the modulus of elasticity
E is based on bending test results. The effect of time (relaxation) is not
taken into account.
Design Parameters Design parameters depend on the material type and the design code.

AxisVM provides preloaded cross-section libraries, that contain the most
frequently used steel shapes and concrete cross-sections, and allow you to
create standard cross-section property sets that you can use over and over
again in many different models. The libraries includes products of
manufacturers worldwide.
For the description of the Table Browser see 2.9 Table Browser.
F
The Undo function does not work when libraries are modified.

Create a new library

You can create a custom cross-section library by the File / New Cross-Section
Table command in the Table Browser. You have to specify library name, library
file name and a cross-section type. Standard and custom cross-section library
files (*.sec) are stored in the folder where the application is stored.

(*) If first and second principal axes are the local y and z axes values
with (*) appears with indices y and z.

82 AxisVM 8+Release 4

Table properties

Import/Export
values

Copy/Paste a cross-
section

Add/Modify /
Delete a cross-
section
Custom library properties can be modified by the File / Cross-Section Table
Properties command in the Table Browser.
Custom library properties can be deleted by the File / Delete Cross-Section Table
command in the Table Browser.

You can import and export numerical values in libraries as dBaseIII files by
File / Import dBase file.

You can copy and paste cross-sections with their full graphical description
within the Table Browser. Numerical data exchange with other applications is
supported via clipboard.

You can add a new cross-section to any custom or standard library by
Edit / New Row (or by pressing [CTRL+INS] or the toolbar button) in the Table
Browser and entering field values.
You can also call the Cross Section Editor to specify cross-section data.
Use Edit / Design New Cross-Section (or [CTRL+G]) to add a new cross-section and
Edit / Modify Cross-Section (or [CTRL+M]) to modify an existing one.
Changing any dimension of a standard shape AxisVM automatically
recalculates all cross-section parameters and updates the graphics.
You can delete a cross-section with the aid of deletion icon or by pressing
[CTRL+Del].
See description of the cross-section editor in section 3.1.13.1.
F
Cross-section libraries contain the values of the warping inertia Iω used in the
Steel Design module.

The property values in standard libraries are taken from manufacturers’ data-
bases. You must verify them before use.

The table below shows the shape and reference coordinate system of the cross-
sections. The properties that were not published by the manufacturers were
calculated.

User’s Manual 83

Cross-sections

In the calculation of cross-
section properties and dis-
playing the cross-section the
rounding (corner and fillet)
radii (r
1
, r
2
, r
3
) are also taken
into account.

The explanation of the these
radii, height, width, wall-thick-
nesses and diameters can be
seen in the schematic diagrams
below.
The Cross-section Library contains the following type of cross-sections:
Steel cross-section

Concrete cross-
sections
The concrete cross-sections are listed starting from the size 20x20 to size 80x80
cm in steps of 2 and 5 cm.

User’s Manual 85

3.1.13.1. Cross-Section Editor

The Cross-section Editor allows you to edit thin and thick walled cross-sections.
You can use parametric circular, rectangular, ring and polygonal shapes, or any
shape listed in the cross-section libraries to edit composite cross-sections.
The shapes used to build a new cross-section are referred to as components,
and have to be of the same material.
You can translate, rotate, mirror, copy or move the selected components at any
time during the editing. When a component is placed to its location
graphically, the principal axes and the cross-sectional properties of the
composite cross-section are computed.
You can use keyboard commands the same way as in main editing windows.

The OK button exits and closes the cross-section editor window, and saves your
current cross-section into the cross-section table of your model with a name
you specify.

Cross-section editor is on the toolbar of the Cross-section Library and can also
be launched from the line element dialog. See... 4.9.6 Line Elements
The editor can be used when creating a native model from an architectural
model through the IFC interface. See... 4.9.18 Creating model framework from
an architectural model

Editor Keys See... 2.5 Using the Cursor, the Keyboard, the Mouse

Toolbar Most important functions are available from the toolbar.

Prints the cross-section. See... 3.1.9 Print

Adds the image of the cross-section to the Gallery.
See… 3.2.8 Saving drawings and design result tables

Undoes the last operation.

Redo the operation which was undone.

Copies the image of the cross-section to the Clipboard.

From Cross-section
Library

Loads a cross-section from the Cross-section Library. Only thick or thin-walled
cross-sections are available depending on the cross-section editor tab position.

From DXF file

Contour of thick walled cross-sections can also be imported from a DXF file.

Stress-points

You can specify the points you want to calculate stresses for. The default stress-
point is the center of gravity. You can specify up to 8 stress-points for each
cross-section.
When applying a move command the stress-points can also be moved.
F
Stress calculations are performed at the specified stress-points only. If you don’t
specify any stress-points, stress will be calculated in the center of gravity only.
It means that no bending stress will appear.

Icon bar Editor functions and settings can be found on the Icon bar on the left.
The behaviour of the Icon bar is the same as that of the main Icon bar.
See... 2.15 Icon bar.
The only difference is that this Icon bar can be moved above the menus at the
top or at the bottom but it is not dockable.

86 AxisVM 8+Release 4

Thin-walled cross-
sections

A component belonging to the thin-walled category can be added to your
cross-section.

Base-point You can select a base-point to each cross-section component, that allows you to
position the component during editing, depending on its shape and final
location within the composite cross-section.

Standard shapes can also be defined parametrically. In this case the following
parameters has to be defined in the dialog:
Manufacturing
process
There are three options (rolled, welded, cold formed.)
Dimensions Values depending on the type of the cross-section (height, width, thickness,
corner/fillet radius, diameter etc.).
Rotation Lets you define a rotation by angle α. The default value is 0.

I shape
,
Wedged I shape

Definition of an I or wedged I shape by its height, width, web and flange
thicknesses and a fillet radius.

User’s Manual 87

Asymmetric I shape

Definition of an asymmetric I shape by its height, width, web and upper /
lower flange dimensions.
Rectangular

Definition of a rectangle by its parameters b (width), v (thickness), and α, with
b>v.

Pipe

Definition of a pipe by its parameters d (outside diameter), and v (thickness).
The centerline is considered as the contour of a closed domain, which is
displayed with a dashed line.

Other shapes
, ,
, ,
Definition of cross-sections by height, width, thickness and in the case of rolled
or bended cross-sections by the corner/fillet radius.

Polygonal

Definition of a polygonal shape.

Before the definition the position of the
control line of the segment can be selected:

1. left side
2. center line
3. right side
R parameter : Rounding (corner and fillet)
radii

88 AxisVM 8+Release 4

Arc shape

Definition of an arc shape by its diameter, central angle and thickness.

Delete Using the [Del] key you can invoke the Selection Icon Bar, and select the
components you want to delete.
When deleting a component the stress-points will also be delete.

Stress-point Deletes the selected stress-points.

F
You cannot delete the default stress-point (the center of gravity).

Options Lets you set the grid size, cursor step, and the zoom factors.

Thick-walled
cross-sections

Rectangular

Definition of a rectangle by its parameters b (width), h (height), and α.
Circular, Semi-
circular ,
Definition of a circular or semicircular shape by its diameter and α.
I shape

Definition of an I shape by its parameters a1, a2, a3, b1, b2, b3, and α. (a1, a3),
(b1, b3). Parameters can be set to 0, allowing the creation of T, U, L shapes.
Polygonal

Definition of a polygonal shape by drawing a polygon.

Insert a vertex

Insertion of a new vertex on the contour of the cross-section. Shape of the
cross-section can be changed by dragging a vertex by the mouse.

Contour

If the Contour button is down the cross-section can be defined. If the Hole
button is down a hole can be specified.

Hole

You can specify a hole in rectangular, circular, and closed polygonal shape
components. The hole can be rectangular, circular, and closed polygonal.

User’s Manual 89

Delete
Using the [Del] key you can invoke the selection window, and select the
components you want to delete.
When deleting a component, the stress-points will also be deleted.

Polygon Deletes the selected components.

Stress-point Deletes the selected stress-points.

F
You can not delete the default stress-point (from the center of gravity).

Options Lets you set the grid size, cursor step, and the zoom factors.

Shear deforma-
tions
For beam elements the shear deformations are not taken into account even if
the cross-section was entered with nonzero for the shear area.
The shear areas are used by the rib element and must be positive nonzero
values ( 0 ≠
y
A and 0 ≠
z
A ).
In the steel design module, the shear areas are calculated according to the
corresponding design code, instead of using the values entered here.

ρ = shear factor
Where:
y
x
y
A
A
ρ
·
z
x
z
A
A
ρ
·

3.1.14. Exit
[Ctrl]+ [Q] Exits the program.

3.2. Edit

User’s Manual 91

3.2.1. Undo
[Ctrl]+[Z]

Undoes the effect of the previous commands. To undo a sequence of actions
(more levels), click the down arrow next to the Undo icon, and then select the
actions you want to undo based on the time or type of the commands.
You can set the number of undo/redo levels (maximum 99) in the Main
menu/Settings dialog box.
3.2.2. Redo

[Shift]+[Ctrl]+[Z]

Undoes the undo command or goes forward to reverse one or more undo
commands. You can select the actions you want to redo based on the time or
type of the commands.

3.2.3. Select All
• [Ctrl]+ [A]
See... 2.15.1 Selection

3.2.4. Copy
• [Ctrl]+ [C]
Copies the drawing of the current graphics window to the clipboard.

3.2.5. Delete
[Del]
Deletes the selected entities. If no elements are selected it brings up the
Selection icon bar and then the Delete dialog window.
Lets you delete the selected geometric entities.
To delete:
1. Select the geometric entities to be deleted. You can select the entities
by holding the [Shift] key pressed while you click on the entities with
the left mouse button or use the Selection Icon Bar.
2. Press the [Del] key. If there is no selection, the selection toolbar appears
and objects can be selected for deletion. See... 2.15.1 Selection.
3. Enable the check-boxes of the entities you want to delete.
4. Press the OK button, to finish and close the dialog window.

In the dialog window the check-boxes are active or inactive according to the
contents of the current selection set (intended for deletion).

92 AxisVM 8+Release 4

Geometry Lets you select geometric entities for deletion. Deleting geometric entities that
have assigned finite elements, will result in the deletion of its finite elements
and of the associated loads.

Elements Lets you select finite elements for deletion. Deleting finite elements will not
delete the respective geometric entity, but will delete the loads.

References Lets you select references for deletion. All finite elements that use the deleted
references, and the associated loads will be deleted too.

Mesh Lets you remove mesh from domains.

R.C. Design Lets you select the reinforcement parameters attached to the selected elements
for deletion.

Steel design Lets you select the steel design parameters attached to the selected elements
for deletion.

Add drawing to
Gallery [F9]
You can save drawings from AxisVM in many different contexts: you can save
AxisVM main windows, beam displacement and internal forces diagrams, steel
design results, nonlinear calculation results, reinforced concrete column and
beam design diagrams, bolted joint diagrams. In case of a divided view you
can select to save all windows or the active one only.

F
Drawings Library is another way to store diagrams. While Gallery contains
static image files, the Drawings Library uses associative drawings following
changes in the model. See... 2.13 Drawings Library

User’s Manual 93

Which file format to
use?
Bitmap formats (.BMP, .JPG) store the pixels of the diagram, so Windows
metafiles provide higher resolution when printed. JPG is a compressed format
with a slight loss of quality but these files are much smaller than BMPs.

Windows metafiles (.WMF, .EMF) store a series of drawing commands so they
can be scaled and printed in any size in the same quality. However if you
choose hidden line removal or a rendered view drawn by OpenGL technology
metafiles will contain only bitmaps. To get a high resolution rendered view
print the picture directly.

Drawings will be saved to a subfolder Images_modelname automatically created
under the folder of the model file. These pictures can be inserted into a report.
Do not modify the name of the subfolder Images_modelname.

3.2.9. Weight Report
[F8]
The weight of the entire model, selected elements or details can be listed in
tabular form per material, per cross-section or surface type.

3.2.10. Find structural members

AxisVM handles line elements as structural members. It means that Meshing of
line elements on the Mesh tab creates finite elements but the line elements them-
selves are not divided. The Find structural members menu command joins adja-
cent line elements into a single element until a breaking point is found.
A breaking point is defined by different local x or z directions, different mate-
rial, cross-section or eccentricity, end release or a domain boundary. Line ele-
ments must be on the same line or on the same arc.

3.2.11. Break apart structural members

The Break apart structural members menu command breaks apart line elements
created with the Find structural members command.

3.3. Settings

94 AxisVM 8+Release 4

3.3.1. Display

Symbols See... 2.15.13. Display Options
[Ctrl]+ [Y]

Labels See... 2.15.13. Display Options
[Ctrl]+ [L]

Switches See... 2.15.13. Display Options
[Ctrl]+ [D]

3.3.2. Options

See... 2.15.14. Options

3.3.3. Layer Manager
[F11]

The Layer Manager allows you to manage AxisVM layers, imported DXF
or ArchiCAD layers. While only one ArchiCAD layer can be imported, multiple
DXF layers are allowed.
If no AxisVM layers are defined AxisVM automatically creates a new layer for
dimension lines with the name Dimensions.

On the left side of the Layer Manager dialog a tree view of the available layers
is displayed. If you select (highlight) a DXF layer in the tree, you can modify its
properties in the right side (Name, Color, Style, Size). If you select the main
DXF file entry of the tree, you can modify all the DXF layers at a time.
Properties of AxisVM structural layers cannot be modified.

User’s Manual 95

Apply to All: When using this button, a dialogue window will allow you
to select the items in the DXF layers that will have their properties set based on
the layer’s settings.

The visibility of the layers or DXF files can also be set by clicking on the bulb
or cursor symbol next to the layer or file name.

New AxisVM Layer Creates a new AxisVM layer. You can set the layer’s name, color, line style and
size.

Delete More than one layer or group can be selected and deleted by the [Del] key.

Sets the Design Code to be used in case
of code specific tasks. Changing Design
Code changes the method of calculating
critical load combinations therefore all
load group parameters but safety
factors will be deleted. Seismic analysis
parameters and seismic load cases will
also be deleted. As material properties
and certain reinforcement parameters
are not the same in different codes it is
recommended to revise the values you
have specified.

3.3.6. Units and Formats

Lets you configure the units (SI and/or Imperial) and formats of variables used
throughout the program (number of decimals used for displaying or
exponential format). You can use predefined sets as the SI set, or create and
save your own custom sets.

96 AxisVM 8+Release 4

3.3.7. Gravitation

Lets you set the gravitational acceleration
constant and the direction of gravitation
as one of the global coordinate directions

3.3.8. Preferences

Data Integrity

Recent file list

Lets you set the number of recently opened AxisVM model files listed in the
bottom of the File menu, and set if you want the last edited file to be opened
at startup. The welcome screen (See... 2.2 Installation) will be shown on
startup if the show welcome screen on startup checkbox is checked.

User’s Manual 97

Save

Auto Save option
To make sure that you do not lose your work, select the Auto Save option by
the check box. In the Minutes box, enter the interval at which you want to
automatically save the opened model (1-99 minutes). You must still save the
model when you exit.
A model that is saved automatically is stored in the default temporary folder
of the operating system (by default it is c: \ Documents and Settings \ username \
Local Settings \ Temp) as ~modelname.avm until you perform a save command.
When you have to restart AxisVM after a power failure or due to any other
problem that occurred before you saved your work, AxisVM can recover it
from the temporary file stored in the above folder under the name
$modelname.avm.
Create Backup Copy
If this checkbox is checked and a model is saved after making changes a
backup copy is automatically created from the previous state of the axs file.
Name of the backup file is modelname.~AX.
Save derivative results
If this checkbox is checked stresses, envelopes, critical combinations and
design results will be saved as well.

Undo

You can undo your last actions. You have to specify the maximum number of
actions you want to undo. This number must be between 1 and 99.

GroupUndo

The Group Undo option allows you to undo the effects of complex
commands in a single step.

Network time-out

In case off network hardware protection keys, if in a time period set here
there is no activity (checks) with the key, the current AxisVM session is
closed.
Disconnecting may also happen in a situation when you get a phone call and
you do not use the program for a time longer than the network time-out.
If another user asks for access to the key the server gives a license to him/her
and when you try to continue your work the program displays an error
message and halts at the next key check.

Lets you change the typeface and size of the fonts that are used when
displaying your model and the Floating Palettes. Click white sample area to
get to the font selection dialog.
Default settings can be restored by pressing the button on the right.

Edit

Two general editing parameters can be set on this panel.

Circle Closing
Angle
Parameter for drawing arcs. If the center angle of the arc is smaller than this
angle or it is closer to 360° than this angle then a whole circle will be drawn.

Projection line to
workplane
Display of projection lines can be turned on/off. Its shows the distance of the
cursor from the current workplane.

Meshing

Mesh management

One of the following mesh management methods can be chosen.
Remove and create mesh automatically
Any editing performed on a domain deletes its mesh. When launching the
analysis missing meshes will be recreated based on the meshing
parameters of the domain.
Keep mesh editable
Meshes can be edited manually.

User’s Manual 99

Contour division
method

Uniform mesh size
Meshes will be generated according to the user defined element size
regardless of the shape of the domain (least number of finite elements).
Adaptive mesh size
Takes the shape of the domain into consideration and creates a better mesh
by increasing mesh density wherever it is necessary.

Default mesh size When defining meshing parameters for a domain for the first time this value
will appear by default.

Toolbar

Displaying toolbar If Horizontal toolbars expanded is chosen, all icon appears in a row.
Separator lines indicate different groups of functions.
If Flyout toolbars is chosen, different functional groups will be represented
by a single icon. Clicking the arrow in the right bottom another toolbar flies
out showing different tools.

Pet palette position Pet palette position can be:
Relative
Specify the horizontal (dx) and vertical (dy) distance from the operation in
pixels.
Appear in the latest position
Pet palette appears in its latest position.

Arcs are displayed as polygons. Set the display resolution here. The finer the
resolution the closer the polygon will get to the arc. This parameter affects
drawing only and is not related to the precision of the analysis.

100 AxisVM 8+Release 4

Analysis

At the beginning of the analysis AxisVM divides the system of equations into
blocks according to the available physical and virtual memory. It makes
analysis more efficient but can considerably slow down other applications.
Set the amount of virtual memory you let AxisVM use during the analysis
here.
Using a single
thread /
Using multiple
threads

Using multiple threads makes AxisVM run analysis on multiple threads.
To make the most of this option it is recommended to use a processor with
HT-Hyperthread or DualCore technology.
Multi-threading improves speed of calculation. Improvement depends on
the available memory and the model size. Linear analysis will be 1.5 times
faster, while vibration analysis can be 4 times faster.
Folder for temporary
files during analysis
You can specify the location of temporary files during analysis.
Select any of these options :

Table layout If Allow multiple columns is checked, narrow report tables will be printed in a
multi-column layout to reduce the space required. Minimum number of rows
per column can be specified to avoid column breaks for short tables.

User’s Manual 101

Update

Search for updates
on each startup
If this option is turned on AxisVM searches for live internet connection on
each startup. If it finds one, searches for program updates. If a new release is
available it shows a message and let the user download the update.

AxisVM
Web Update
Click the button to get to
the AxisVM Web Update
Wizard which is a guide
to the download process.
If download is complete
and the Update the pro-
gram option is checked
on the last page, the pro-
gram quits and start the
installation of the new
release.

3.3.9. Toolbars to default position
The moveable Icon bar will get back to the left side. All flyout toolbars
undocked and dragged to a new position will get back to the Icon bar.

3.4. View

Front view
[Ctrl]+ [1]
See... 2.15.3 Views

102 AxisVM 8+Release 4

Top view
[Ctrl]+ [2]
See... 2.15.3 Views

Side view
[Ctrl]+ [3]
See... 2.15.3 Views

Perspective view

[Ctrl]+[4]
See... 2.15.3 Views

Setting
Perspective View
See... 2.15.3 Views

Work planes

See... 2.15.4 Workplanes

Zoom in
[Ctrl]+ [/], [+]

See... 2.15.2 Zoom

Zoom out

[Ctrl]+ [Shift]+[/],[-]

See... 2.15.2 Zoom

Zoom to fit

[Ctrl]+ [W]

See... 2.15.2 Zoom

Pan

See... 2.15.2 Zoom

Rotate

See... 2.15.2 Zoom

View undo

[Ctrl]+[

See... 2.15.2 Zoom

View redo

[Ctrl]+]

See... 2.15.2 Zoom

Wireframe

See... 2.15.6 Display Mode

Hidden line
removal

See... 2.15.6 Display Mode

Rendered

See... 2.15.6 Display Mode

Rendering
options...

See... 2.15.6 Display Mode

Wireframe cross-
sections
In rendered mode thin walled cross-sections will be displayed only with mid-
planes.

Actual
cross-sections
In rendered mode thin walled cross-sections will be displayed as solid objects
with their actual shape.

Wireframe while
dragging
If it is switch on, the program display the wireframe of the model during the
rotation or pan.

No labels while
dragging
If this option is turned on, labels are not drawn during rotation or panning.

User’s Manual 103

3.5. Window

3.5.1. Property Editor
Property Editor provides the fastest way to change properties of the selected
nodes, elements or loads. All changes are made immediately. If the selection
contains different elements it is possible to change their common properties
(e.g. after selecting trusses, beams and ribs their material and cross-section will
be editable).
If result or design tabs are active the values are read only.
In certain fields regular mathematical expressions are also accepted.
Available operators and functions are:

Properties are displayed in a tree-like structure. Clicking a [+] or [–] symbol
before the property name expands or collapses a list of sub-properties.
If the (...) button appears in a line the property can be changed using a
separate dialog.

>> If the (>>) button appears in a line the property can be picked up from
another element by clicking it.

Property Editor can be used to modify data but also to select and filter
elements with the same property.

104 AxisVM 8+Release 4

Filter

Selecting a property and clicking the filter button you can select all the
elements having the same property value.
Example: changing an existing cross-section in the whole structure.
Selecting the cross-section property of a rib element you can select all rib
elements with this cross-section then change their cross-section property
of them.

3.5.2. Information Windows

Lets you set the display of the Info, Coordinate, and Color Legend Windows to
on or off.
See... 2.17 Information Windows

3.5.3. Background picture

The submenu makes several options available. An automatically fitted back-
ground picture can be loaded to the main window of AxisVM to show the
model in its future environment. Load Background Picture... submenu item
or [Ctrl+B] opens a file browser dialog, Reload Background Picture shows the
most recently used picture files. In multi-window mode each window can
have its own background picture.

Picture in the active window can be turned on and off by clicking Display or
by [Ctrl+Alt+B].
Save Background Picture saves the picture in the active window into a file.
If the aspect of the picture differs from the window aspect Shift Background
Picture makes it possible to drag the background to a new position. Remove
Background Picture removes the picture in the active window.
Background pictures are saved into the AXS file.

After loading a background picture the model can be set to an appropriate
view by zooming out, zooming in, panning, rotating and setting the
perspective.

3.5.4. Split Horizontally

Inactive graphics
window
Active graphics
window
User’s Manual 105

Splits the graphics window horizontally into two parts. The display settings of
each window can be set independently.
You can maximize or minimize or restore the graphics windows by using the
buttons at the top-right of the windows.

3.5.5. Split Vertically

Splits the graphics window vertically into two parts. The display settings of
each window can be set independently.
You can maximize or minimize or restore the graphics windows by using the
buttons at the top-right of the windows. Different load cases can be set in each
window but only when displaying results.

3.5.6. Close Window

Closes the current graphics window.

3.5.7. Drawings Library

The Drawings Library contains drawings saved in the program. Drawings are
not saved pictures but instructions how to draw a view of the model or parts of
it including multi-window settings. Drawings can be reloaded to restore saved
view and display settings. Including drawings into a report makes it easier to
update the report when the model has changed and recalculated as drawings
will be updated automatically like tables.
Drawings Library can store displacement, force, stress diagrams of line
elements, diagrams of steel and bolted joint design, punching analysis,
reinforced concrete column check and beam design in an associative way.

Clicking the arrow beside the tool button an
existing drawing can be selected from a pop-
up list, restoring its view and display
settings.

Loads a chosen drawing to the active window.
(available in multi-window mode only)

Loads a chosen drawing to the window.

Restore result components
If this option is checked loading a drawing displaying results restores the
result component as well and sets the appropriate tab (Static, Vibration, etc.).
If this option is unchecked loading a drawing does not restore the result
component and the tab.

OK Saves the changes and loads the selected drawing.
Cancel Does not save changes.

3.5.8. Save to Drawings Library

User’s Manual 107

By clicking this tool button one or more drawings can be saved into the
Drawings Library. If the current drawing is, a Found in the Drawings Library
label is displayed in the dialog. It can be overwritten or the drawing can be
renamed. Multiple drawings button opens additional options. Load cases, load
combinations (and result components if results are displayed) can be chosen.
AxisVM creates all combinations (i.e. all selected result components in all
selected load cases) and saves them into the Drawings Library with the current
view and display settings.
Clicking the Drawings Library button displays the Dawings Library dialog.

3.6. Help

Lets you use the online help of AxisVM. To get context-sensitive help
information about the operations related to a dialog box press [F1].

3.6.1. Contents
[F1]
Opens the table of contents of the help, and allows access to the topics you are
interested in.

3.6.2. AxisVM Home Page

Visits AxisVM Home Page using the default Internet browser.

3.6.3. AxisVM Update

Launches the AxisVM Web Update Wizard. See... 3.3.8 Preferences

3.6.4. About

Tells you more information
about your AxisVM program.
You can use this command
to determine the ver-
sion/release number, confi-
guration, serial number and
time limit of your AxisVM
version.

3.6.5. Release information...
Latest release information and history of fixes and new developments.

108 AxisVM 8+Release 4

3.7. Main toolbar

3.7.1. New

See... 3.1.1 New

3.7.2. Open

[Ctrl]+[O]
See... 3.1.2 Open

3.7.3. Save

[Ctrl]+[S]
See... 3.1.3 Save

3.7.4. Print

[Ctrl]+[P]
See... 3.1.9 Print

3.7.5. Undo

[Ctrl]+[Z]
See... 3.2.1 Undo

3.7.6. Redo

[Shift]+[Ctrl]+[Z]
See... 3.2.2 Redo

User’s Manual 109

3.7.7. Refresh

[Ctrl]+[R]
Refreshes the drawing in the windows.

3.7.8. Layer Manager

[F11]
See... 3.3.3 Layer Manager

3.7.9. Table Browser

[F12]
See... 2.9 Table Browser

3.7.10. Report Maker

[F10]
See... 2.10 Report Maker

3.7.11. Drawings Library

See in detail... 3.5.7 Drawings Library

3.7.12. Save to Drawings Library

See in detail... 3.5.8 Save to Drawings Library

110 AxisVM 8+Release 4

This page is intentionally left blank.

User’s Manual 111

4. The Preprocessor
The preprocessor lets you create or modify the geometry of the model,
in a completely visual way. The advanced Visual Modeling feature allows
quick and reliable modeling and design.
This chapter introduces the AxisVM modeling commands (geometry gene-
ration, element/mesh generation, and load case/combination definition).

4.1. Geometry
Geometry commands let you interactively and graphically create the model
geometry in 3D.
The model geometry is defined by nodes (points), mesh lines (lines) between
nodes, and surfaces (triangular or quadrilateral) created from three or four
appropriate lines. Later you can define finite elements based on the geometry
constructed here.

In the case of surface structures (plates, membranes, or shells) the mesh
consists of quadrilaterals that represent the median plane of the elements.

In the case of frame structures (beams or trusses) the mesh consists of the axes
of the elements.

112 AxisVM 8+Release 4

4.2. The Geometry Editor

When AxisVM starts, the graphical user interface is ready for geometry editing.
In case of a new model X-Y, X-Z or perspective view can be set as the default
view. In case of an existing model the latest view settings will be loaded.
Using the horizontal icon toolbar at the top of the graphics area you can apply
various commands to construct geometry meshes describing the geometry
of your finite element model. See...4.8 Geometry Toolbar

Using the vertical icon bar on the left you can apply commands that change
the display of the model, and can configure the working environment of the
editor. See...2.15 The Icon

4.2.1. Multi-Window Mode
When the model is complex, it is useful to display different views of the model
simultaneously on the screen. AxisVM allows you to split the graphics area
horizontally or vertically. Each newly created graphics window has its own
settings, and allows the independent display of the model views. This feature
is also useful when interpreting results.
You can access split commands from the Window menu.

Split horizontally Splits the active graphics window horizontally into two equal parts.
The top window will become the active window.

See... 3.5.4 Split Horizontally

Split vertically Splits the active graphics window vertically into two equal parts.
The left window will become the active window.

See... 3.5.5 Split Vertically

Close Window Closes the active window if there are more than one graphics windows in use.
The new default window will be that in which you previously worked.

You can change views during any editing command.
F
In the perspective view some editing commands cannot be used, or are limited in
use.

Context sensitive
help message
Status window

Color legend window

Pet palette
cursor
Moveable Icon bar
Graphics
area

Property
Editor
Speed buttons

Pop-up
rowicon
Coordinate
window

Perspective Toolbar
Top menu bar

Model name and location path

User’s Manual 113

4.3. Coordinate Systems
AxisVM uses different coordinate systems, to describe the model. The global
coordinate system is used to describe the model geometry. Local coordinate
systems are mainly used in the element definitions. The local systems are
usually defined by the element geometry and additional references. AxisVM
denotes the axes of the global system with capital letters, and the local axes
with small letters.
The geometry can be created using Cartesian, Cylindrical or Spherical
coordinate systems.

See... 4.3.2. Polar Coordinates

4.3.1. Cartesian Coordinate System

Base coordinate
system
AxisVM uses Cartesian coordinates to store geometry data.
AxisVM uses the right-hand rule exclusively to define the positive directions
of axes and rotation. The illustration below shows the positive directions of
the axes and of rotation according to the right-hand rule.

Global and relative
origo
A new model uses the view selected in the New Model dialog
(see... 3.1.1 New Model). The origin of the coordinate system is shown by a
blue X initially located at the left bottom corner of the editor window.
A fixed (X, Y, Z) and a relative (dX, dY, dZ) global system are used to locate
points (nodes) in your model. The origin of the relative system can be
moved anywhere (using [Alt]+[Shift] or [Insert]), at any time during modeling.
The Coordinate Window displays either the fixed or the relative global
coordinates according to its current settings. If the relative mode is selected,
the denotation of axes becomes dX, dY, dZ.
With the help of the Coordinate Window, and according to the movement
of the relative origin you can make measurements on the model (distances,
angles).
The nodal displacements and mode shapes refer to the fixed global system.

F
In the X-Y and Y-Z views the third axis (normal to the view’s plane)
is oriented toward you. As a result, when a copy is made by translation with
a positive increment about the respective third axis, the copies will be placed
in front (toward you). The opposite occurs with the third axis in the case of an
X-Z view is oriented in the opposite direction.
See...4.9.17 References

114 AxisVM 8+Release 4

4.3.2. Polar Coordinates
In addition to the Cartesian global coordinate system, you can use either
a cylindrical or a spherical coordinate system. One of the polar coordinate
systems can be selected through its corresponding radio button
in Settings / Options / Editing / Polar coordinates.

In the Coordinate Window three variables will be displayed depending on
selection:

Cylindrical
h: the value measured from the view plane to a point on the cylinder’s
main axis (that is perpendicular to the view plane) oriented outward
from the screen
r: radius that is the distance on the view plane from the projection of the
point to the cylinder’s main axis
a: the angle between the line that joins the point with the origin and the
horizontal

Spherical
r: the radius, that is the distance from the point to the sphere’s center
(origin)
a: the angle on the view plane between the line that joins the projection
of the point with the origin and the horizontal
b: the angle between the line that joins the point with the origin and the
view plane, which is positive if the point is in front of the view plane
(between the user and the view plane).

Cylindrical Coordinate System Spherical Coordinate System

4.4. Coordinate Window

Displays the current absolute and relative values of the cursor position in the
global coordinate system (Cartesian and cylindrical or spherical).
You can switch between absolute and relative coordinate displays, by clicking
on the letters d in the Coordinate Window. The display of the d letters also
show whether the relative coordinates are enabled or not.

The positive angles, α:

F
The relative switch (delta) can be used together with the constrained cursor
movements.
See... 4.7.4 Constrained Cursor Movements.
User’s Manual 115

4.5. Grid
See in detail...2.15.14.1 Options
4.6. Cursor Step
See in detail...2.15.14.1 Options
4.7. Editing Tools
Editing tools help the work by several features. See... 2.15.14.2 Editing

4.7.1. Cursor Identification
Sets the size of the cursor
identification area (in pixels).

When you position the cursor over the graphics area, AxisVM finds the entity
of the model that is closest to the center of the cursor from among the entities
that are located in or intersect the identification area. The size of the
identification area can be set at Settings / Options / Editing / Cursor identification.

The current shape of the cursor shows what kind of entity was identified.
Depending on entity type, the cursor will have the following shapes:

Node

Mid-side node

Support

Edge hinge

Mesh independent
load

Load polygon vertex

Center of an arc

Arc

Tangent

References

Line

Surface

Intersection

Perpendicular (normal)

Guideline

Domain

116 AxisVM 8+Release 4

Rigid element

Dimension line

In case of Pick up
function

Text box, label

If there are several entities at the same location, the program identifies the first
entity according to the ordering of the list above. If there are multiple entities
of the same type, the cursor will show a double symbol.

F
Use the Coordinate Window to find out which one of the elements was actually
identified.

Background
detection
The cursor can be set to detect the lines on architecture background layers.

4.7.2. Entering Coordinates Numerically
During the model editing, coordinates of the cursor can be specified directly
entering the numerical values into the Coordinate Window. There are two
ways to enter the numerical values:

1. by pressing the corresponding character button on the keyboard
2. by clicking with the left 8 button on the desired coordinate value display
field, and then typing in the value.

If the relative mode is enabled (the letter d is depressed), the coordinates you
enter will define a point from the relative origin.
If contradictory values are entered (in case of a constraint), the last entered
value will update the others.

The relative origin can be moved at any time, anywhere. Therefore when
drawing a line, you can specify its endpoint coordinates relative to different
origins.
F
To draw a line with a given length and direction move to relative origin to the
starting point, enter the angle at d a[°] and enter the length at d r[m] then press
the Enter button.

4.7.3. Measuring Distance
The distance between two points or the length of a line can be measured
by moving the relative origin onto the first point and then identifying the
second point by positioning the cursor over it. In this case the value of dL
in the Coordinate Window is the distance between the points.

The cursor can be moved to a location relative to a reference point by moving
the relative origin onto the reference point, then entering the angle in the
input field da and the distance in the dr input field.

4.7.4. Constrained Cursor Movements
The cursor movement constraints can be customized in the Settings / Options /
Editing dialog. The constrained cursor movements use the following values:

User’s Manual 117

∆α Holding the [Shift] key pressed, the cursor is moving along a line that connects
its current position with the origin, and that has an n*∆α angle, where the
value of n depends on the current cursor position.

Custom α Holding the [Shift] key pressed, the cursor is moved a line that connects its
current position with the origin, and that has an α or α+n*90° angle, where
the value of n depends on the current cursor position.
∆α and α can be set in Settings/Options/Editing/Constraint Angle.

The meaning of origin depends on the d switches of the coordinate palette.
Turning off both the origin will be the global origin. Turning on any of the d
switches the origin will be the local origin.

F
You cannot use ∆α and Custom α constraints in perspective view.
If the cursor is over a line, holding the
key [Shift] depressed, will constrain
the cursor movement to the line and
its extension .

If the cursor identifies a point,
holding the key [Shift] depressed,
makes the cursor move along the line
defined by the point and the relative
origin..

When the cursor identifies a domain or surface element pressing [Shift] makes
the cursor move in the plane of the element.

The icons of Geometry Tools allow you to lock the direction of drawing a line.

See... 2.15.8 Geometry Tools

4.7.5. Freezing Coordinates
You can freeze the value of a coordinate, allowing for better positioning.
A frozen coordinate will not change on cursor motion. Freezing can be
achieved by using [Alt] + [X],[Y],[Z],[L],[R],[A],[B], [H] respectively. A black
rectangle over the coordinate input field shows that the coordinate is frozen.
To cancel coordinate freezing, press the same button combination, that was
used to freeze it or press [Alt]+ [Space].

4.7.6. Auto Intersect
At the intersection point of the lines, a node will be generated and the lines
will be bisected. If surfaces are intersected by lines, they will be split, and the
resulting elements will have the same material and cross-sectional properties
as the original. Set the line intersection options in Settings/Options/Editing/
Auto Intersect. See... 2.15.14.2 Editing

If Auto Intersection is on, surfaces will be divided into smaller surfaces
if necessary. Surface finite elements are also divided and the new elements
inherit the properties and loads of the original element.

Frozen X coordinate
Frozen angle
User’s Manual 119

4.8. Geometry Toolbar

These tool buttons create new geometry or change the existing one..
F
If you are working on parts and Settings / Options / Editing / Auto / Part Manage-
ment option is checked then all the newly created geometric entities will be added
to the active parts.
The geometric entities can be selected prior to applying the geometry con-
struction commands, as well.

4.8.1. Node (Point)

Lets you place new nodes or modify existing ones.
To place a node:
1. Move the graphics cursor to the desired location and press the [Space] key
or the left mouse button (in perspective view you can place nodes only
to special locations).
2. Enter the node coordinates numerically in the Coordinate Window, and
then press [Space] or [Enter] (it works in all views).

You can place a node on a line or surface. If the Settings / Options / Editing /
Auto Intersect check-box is enabled, the line or surface will be divided by the
new node, otherwise it remains independent of the line.
F
If nodes are generated closer to each other than the tolerance specified in Settings /
Options / Editing / Editing Tolerance value, nodes will be merged.

When working on parts with Settings / Options / Editing / Auto / Part Management
turned on all geometric entities created will be automatically added to the active
parts.

4.8.2. Line

The Line Tool is to construct lines or other simple shapes. The line type can be
chosen by clicking on the arrow at the bottom-right corner of the currently
used Line Tool Icon, and then clicking on the desired Line Icon.

The Line Tool offers the following options to
draw simple shapes:

Line

Constructs straight lines by defining their end points (nodes). You must
graphically or numerically (by the Coordinate Window) specify the endpoints
(nodes). The command lets you generate one or more independent lines.
You can cancel the process by pressing the [Esc] key or the right mouse button.
In perspective view lines are drawn on the Z=0 plane by default. To draw lines
in perspective in a different plane workplanes can be used.
See... 0 Workplanes.

Polyline

Constructs a series of connected straight lines (a polyline). You must specify the
vertices.

Exit current polyline by pressing the:
1. [Esc] key
2. [Esc] key a second time will exit polyline drawing mode.
3. 8 right button & Quick Menu/Cancel
4. 8 left button while pointing to the last point (node) of the current
polyline.

After you specified the first corner you can cancel the command by pressing
the [Esc] key. This command is not available in perspective view.

Skewed rectangle

Constructs a skewed rectangle (its corner points (nodes) and edge lines).
You must specify one of its sides (by its endpoints), and then the other side.

After you specify the first corner you can cancel the command pressing
the [Esc] key. In perspective view, you can draw skewed rectangles using only
the existing points.

Polygon

Number of sides has to be defined in a dialog. Polygon has to be defined
by entering a centerpoint and 2 polygon points.

4.8.3. Arc

Draws an arc or a circle. Arcs and circles will be displayed as polygons
according to the Arc resolution set in Settings / Preferences / Display.
[Esc] cancels the command.

Defining an arc by its radius, and starting and ending points.

Defining an arc by three points. The command can be applied in perspective
setting as well.

3rd point
1st point
(central point)
1st point
2nd point
3rd point
arc
2nd point
arc
Endpoint
User’s Manual 121

4.8.4. Horizontal Division

This function creates a horizontal divider line passing through the cursor
position. This line is in a plane parallel with the X-Y, X-Z or Y-Z plane
depending on the actual view (or parallel with the workplane if a workplane is
used). Creates new nodes at the intersections. If finite elements are intersected
new elements inherit properties and loads of the original element.

4.8.5. Vertical Division

This function creates a horizontal divider line passing through the cursor
position. This line is in a plane parallel with the X-Y, X-Z or Y-Z plane
depending on the actual view (or parallel with the workplane if a workplane is
used). Creates new nodes at the intersections. If finite elements are intersected
new elements inherit properties and loads of the original element.

4.8.6. Quad/Triangle Division

Constructs a mesh of quads/triangles over a quad or triangle. Use this
command to generate a macro mesh before applying a finite element mesh
generation command. If the mesh is fine enough, it can be used directly as a
finite element mesh.

Quad-to-quads

Generates an n×m mesh between the
corners of a 3D quad (not necessarily flat,
or with any side lines). You must
successively graphically select the corners
(four points), and specify the number of
segments ( 1
1
≥ N ) between corners 1 and
2, and the number of segments ( 1
2
≥ N )
between corners 2 and 3.

$
The quad and the mesh are displayed with solid grey lines.

If the mesh leads to quad subdivisions that are distorted (have an angle smaller
than 30° or greater than 150°), the quad is displayed with grey dotted lines.
If a quad shape is entered that is not allowed (e.g. concave), the quad
is displayed with red dotted lines.

122 AxisVM 8+Release 4

Quad-to-triangles

$
The command is similar to the quad-to-
quads command, but each generated quad
is divided into two triangles by its shorter
diagonal.
The quad and the mesh is displayed with
solid grey lines.

If the mesh leads to triangle subdivisions that are distorted (have an angle
smaller than 15° or greater than 165°), the quad is displayed with grey dotted
lines.
If a quad shape is entered that is not allowed (e.g. concave), the quad
is displayed with red dotted lines.

Triangle-to-quads

Constructs a mesh between the corners of a
triangle (not necessarily with any side lines).
The mesh will also contain triangles along
the side that corresponds to the first two
corners entered.
You must graphically select the corners
successively (three points), and specify the
number of segments N between corners.

$
The triangle and the mesh are displayed with solid grey lines.

If the mesh leads to quad subdivisions that are distorted (have an angle smaller
than 30º or greater than 150º), or to triangle subdivisions that are too distorted
(has an angle smaller than 15º or greater than 165º), the triangle is displayed
with grey dotted lines.
If a quad shape is entered that is not allowed (e.g. three collinear corners),
the triangle is displayed with red dotted lines.

Triangle-to-triangle

The command is similar to the triangle-to-
quads command, except that each generated
quad is divided into two triangles by its
diagonals which are parallel to the side first
entered.

$
Same as for triangle-to-quads.

User’s Manual 123

4.8.7. Line Division

Lets you create new point (nodes) on the selected lines.
The following input options are available:

By Ratio: Lets you divide the selected lines
into two segments. You must specify the
parameter a of the location of the
inserted node relative to the first node (i).
The parameter a must be between
0 and 1. a=0.5 represents a division
of the selected lines into two equal seg-
ments.

By Length: Lets you divide the selected lines
into two segments. You must specify the
length (d) of the segment corresponding
to the first node (i end). The parameter
d must be between 0 and the total
length).

Evenly: Lets you divide the selected lines into several equal-length segments.
You must specify the number of segments (N).

Uniform by length: Lets you divide the selected lines into several equal-length
segments. You must specify the length of segments (d).

before division after division

If finite elements are divided the new elements inherit properties and loads of
the original elements.

F
If you divide surface edge lines surface elements will be deleted.

4.8.8. Intersect

Divides the selected lines by creating nodes (points) at their intersections.
If finite elements are assigned to the lines, finite elements are also divided and
inherit the properties and loads of the original element..

F
If the Settings / Options / Editing / Auto / Intersect check-box was not enabled in
the dialog window at the time of creating the geometric entity, using this
command you can intersect the selected lines. You can select elements for
intersection beforehand.

4.8.9. Normal Transversal

Creates a connection between to lines along their normal tranversal.

124 AxisVM 8+Release 4

4.8.10. Domain Intersection

Creates intersection lines of
domains and line elements.
After clicking the tool button
select domains to create
their intersection or select
a domain and a line to create
the intersection.

4.8.11. Geometry Check

This function eliminates
extra nodes and lines within
a given tolerance. You can
specify the maximum
tolerance (distance) for
merging points. The default
value is ∆L=0.001 [m].

Points that are closer together than this distance are considered to be
coinciding. The coordinates of the merged points (nodes) are averaged.
The command reports the number of merged nodes/lines.

Select unattached nodes or lines:
If this check-box is enabled, AxisVM will send a warning message
if unattached (independent) parts are encountered.

F
The following case is not identified by the
Check command. To avoid having hiding lines
check Settings / Options / Editing / Auto /
Intersect or click Intersect on the Geometry
Toolbar.

4.8.12. Surface

In any cases when you wish to model surfaces (plates, membranes, or shells)
you have to create a mesh that consists of triangles and convex flat
quadrilaterals. The mesh then can be refined.
The command searches all triangles and quads in the selected mesh of lines.
You must select all surface edges when applying the command. The number
of surfaces detected is displayed in an info dialog.
The reported surfaces are geometry surfaces but not surface elements. You can
make them surface elements by assigning material and cross-section properties
to them.

User’s Manual 125

F
Quads have to be flat. AxisVM takes into account only those surfaces that have
an out-of-plane measurement smaller that the tolerance entered in the Settings /
Options / Editing / Editing Tolerance.

4.8.13. Modify, transform
Lets you modify existing geometric entities.
To modify nodes or lines:
1. Position the cursor over the node/line/centre of surface.
2. Holding the left mouse button pressed, drag the node/line/surface.
3. Drag the node/line/surface to its new position, or enter its new coordinates
in the Coordinate Window, and then press enter or press the left mouse
button again.
F
If multiple nodes and/or lines are selected, the position of all nodes and lines will
be modified.
Fast modify: Clicking a node you get to the Table Browser where you can
enter new coordinate values. If multiple nodes are selected and you click one
of them, all the selected nodes will appear in the table.

Moving selected nodes into the same plane: If the plane is a global one you
can move selected nodes into this plane easily.

1. Click on any of the selected nodes.
2. Select the entire column of the respective coordinate.
3. Use Edit / Set common value to set a common coordinate value.

Using pet palettes

Depending on the type of the dragged element different pet palettes appear
on the screen. Their position can be set in Settings / Preferences / Toolbar.

The last two tool buttons determines the behaviour of connecting arcs.

1. Center angle remains constant.
2. The new arc is defined by the dragged node, the startpoint and midpoint
of the original arc.

Entering node coordinates: Clicking a node the table of nodes appears where
coordinates can be changed. After selecting one or more nodes their
coordinates can be edited in the property editor as well.
Examples of aligning nodes to a plane if this plane is parallel with one of
the global coordinate plane:

Note that some elements like springs and gaps can have nonlinear elastic
stiffness properties that are taken into account only in a nonlinear analysis.
In a linear analysis the initial stiffness is taken into account for the spring
element, and the active or inactive stiffness depending on its initial opening for
the gap element.

4.9.1. Material
Define Materials

Lets you define and save material property sets or load them from a material
library.
If you delete a material property set, the definition of the elements with the
respective material will be deleted.

Browse Material
Library
[Ctrl+L]
The material library contains material properties of civil engineering materials
based on Eurocode, DIN, NEN, SIA and other specifications. The following
parameters are stored:

F
If a material type is deleted all elements made of this material will be deleted.

128 AxisVM 8+Release 4

Material Properties Depending on the type of the finite element you must define the following
material properties:

Displaying and changing material properties is described in 3.1.12 Material
Library.

F In AxisVM all the materials are considered to be linear elastic (Hooke’s Law), and
uniform isotropic or orthotropic (for beam, rib, membrane, plate, and shell
elements).
Some elements can have nonlinear elastic material (truss), or stiffness (support,
gap, link, spring elements).
Nonlinear material models are taken into account only in a nonlinear analysis.
In a linear analysis the initial stiffness is taken into account for the nonlinear
elements.

4.9.2. Cross-Section
Define Cross-
sections

Lets you define and save cross-sectional property sets or load them from a
cross-section library. The beam, truss, and rib elements require a cross-section.
The properties are related to the element’s local coordinate system.
For cross-section properties see... 3.1.13 Cross-Section Library

F
If you delete a cross-section property set, the definition of the elements to which
it was assigned will also be deleted. The lines will not be deleted.

You must enter values for all properties.
Cross section properties are defined in the coordinate system of a truss / beam /
rib element.

User’s Manual 129

4.9.3. Domain

A domain is a planar structural
element with a complex geometric
shape described by a closed polygon
made of lines and arcs. A domain can
contain holes, internal lines and
points.
Polygon vertices, holes and internal
lines must be in same plane.

The following parameters can be assigned to the polygon, hole edges, internal lines and
points of a domain:
point, line, and surface support
rib element
distributed load
dead load
thermal load
nodal degrees of freedom (DOF)

$
A domain is displayed by a contour line inside of the domain’s polygon, with a
color corresponding to the domain’s element type (blue for membrane, red for
plate, and green for shell).

Domains can be defined for floors, walls, and any other complex structural
surface element.
The domain can be meshed automatically.
See... 4.11.1.2 Mesh generation on domain

Define a domain Select lines on the contour of the domains you want to define. If you select
more lines or lines from different planes, AxisVM will find the planes and the
contour polygons of the set. The program applies the parameters you entered
in a dialog window.

Modify a domain Select the domain (click on the contour line of the domain) you want to modify
and make the changes in the dialog displayed.

Delete a domain Press the [Del] button, select the domains (click on the contour line of
the domain) you want to delete and click OK in the dialog.

4.9.4. Hole

Holes can be defined in domains. Holes have to be inside the domain and in
the domain’s plane.
Select the (closed) polygons that are the edges of the holes you want to define.
You can move holes from one domain to another, or change their shape.

$
Holes are displayed by a contour line with the color of the domain in which
they are located.

Domain
1
st
Hole
User’s Manual 131

4.9.5. Domain operations
Domain contours can be changed, cut and a union of domains can be
calculated.

Change domain
contour

1. Click the Change domain contour icon on the toolbar.
2. Select a domain to change. Domain countour will be selected.
3. Change selection to modify domain contour and click OK on the selectioin
toolbar.

Before After

F
Domain properties (material, thickness, local system) will be retained but the
existing mesh will be removed.

If loaded areas are removed from the domain, loads will automatically be
removed.

Union of Domains

Union can be created from adjacent domains with matching properties (same
thickness, material, local system).
1. Click the Union of domains icon on the toolbar.
2. Select the domains and click OK on the selection toolbar.

Before After

Cut a domain

To cut a domain along en existing line:
1. Click the Cut of a domain icon on the toolbar.
2. Select the domain.
3. Select the cutting line and click OK on the selection toolbar.

Before After

132 AxisVM 8+Release 4

4.9.6. Line Elements
Line elements are defined and modified in a common dialog. After choosing
the element type specific truss / beam / rib element parameters can be set.
Line elements are handled as structural members and not as finite elements.
Meshing a line element divides a beam or a rib into finite elements. Existing
line elements can be joined to form a single element if the geometry and their
properties allow it. (Edit / Find structural members). Numbering, labeling, listing
functions will consider it to be a single structural member. Structural members
can be broken apart by Edit / Break apart structural members) See... 3.2.10 Find
structural members, 3.2.11 Break apart structural members

Truss

Truss elements can be used to model truss
structures.
Trusses are two node, straight elements
with constant cross-section properties
along the truss length. A maximum of
three translational degrees of freedom are
defined for each node of the elements.
The elements are pin-ended (spherical
hinges).

Axial internal forces N
x
are calculated for each truss. The variation of the axial
force is constant along the element.
i denotes the truss end with the lower node index (first node). By default the
element x axis goes from the node (i), to the node (j). It can be changed
by selecting the other orientation from Local x Orientation.

Define You must select the lines to which you want to assign the same material and
cross-sectional properties in order to define truss elements.
If elements of different type are selected element definition will be activated.

Defining materials
and cross-sections
Materials and cross-sections can be selected from built-in libraries or from a list
of the materials/cross-sections already defined.

Allows browsing of the material library to assign a material to the element.
The material selected will be added to the material table of the model.

Allows browsing of the cross-section library to assign a cross-section to the
element. The cross-section selected will be added to the cross-section table of
the model.

Launches the Cross-section Editor. The cross-section created in the Editor will
be registered in the list of model cross-sections.

Local x Orientation Local orientation of the beam can be changed. The options are: from i to j or
from j to i or automaticaly. Automatic orientation is based on the endpoint
coordinates
i à j : local x axis is directed from the end node with a lower number to the
node with the higher one
j à i : local x axis is directed from the end node with a higher number to the
node with the lower one
Cross-section:
In the calculation of the element stiffness, only the cross-sectional area
A
x
is considered from the cross-sectional properties.

Local z Reference A reference point can be assigned to define the element orientation.
This allows a correct display of the cross-section on the screen. In case of
selecting Auto the reference(s) will be set by the program. Affects only the
display of references. See... 4.9.17 References

Reference angle

Rotation of cross-sections is made easy by the reference angle. The automatic
local coordinate system (and the cross-section) can be rotated around the ele-
ment axis by a custom angle. If the element is parallel with the global Z direc-
tion, the angle is relative to the global X axis. In any other case the angle is rela-
tive to the global Z axis.

Nonlinear
parameters
In a nonlinear analysis you can specify that a truss has stiffness only if it is in
tension or compression. You can optionally enter a resistance value as well.
A nonlinear elastic behavior is assumed for the nonlinear truss elements.
F
The nonlinear parameters are taken into account only in a nonlinear analysis.
The initial elastic stiffness of a truss element is taken into account if a linear
static, vibration, or buckling analysis is performed, disregarding any nonlinear
parameter entered.
Beam

Beam elements may be used to model frame structures.
Beams are two-node, straight elements with constant or variable (linearly
changing) cross-section properties along the beam length. A reference point is
used to arbitrarily orient the element in 3-dimensional space (to define the
local x-z plane). A maximum of three translational and three rotational degrees
of freedom are defined for each node of the elements. The ends of the ele-
ments can have arbitrary releases.
Three orthogonal internal forces, one axial and two shear (N
x
, V
y
, V
z
), and
three internal moments, one torsional and two flexural (T
x
, M
y
, M
z
) are cal-
culated at each cross-section of each element. The variation of the internal
forces along the beam are: constant axial force, constant torsion, constant shear
forces and linear moments.
The displacements and internal forces are calculated at intervals of at least 1/10
of the element length.
134 AxisVM 8+Release 4

i denotes the beam end with the
lower node index (first node).
By default the element x axis goes
from the node (i), to the node (j).
It can be changed by selecting the
other orientation from Local x
Orientation.

Material, cross-
section, local x
orientation
Defining material, cross-section and local direction X are similar to truss
elements.

Automatic reference

The reference vector will be generated by the program according to the section
4.9.17 References.
The orientation of the local x axis of the element can be reversed or can be set
to Auto which means that local x directions will be set automatically based on
the beam end coordinates.

Reference angle

Rotation of cross-sections is made easy by the reference angle. The automatic
local coordinate system (and the cross-section) can be rotated around the ele-
ment axis by a custom angle. If the element is parallel with the global Z direc-
tion, the angle is relative to the global X axis. In any other case the angle is rela-
tive to the global Z axis.

$
The beam elements are displayed on the screen as blue lines.

End releases

You can specify releases that remove the connection between the selected
elements’ degrees of freedom (in the local coordinate system) and the nodes.
The end-releases are set by a six code set for each end. Each code corresponds
to one internal force component. By default the beam ends are considered
rigidly connected (all codes are of rigid connection) to the nodes. Setting a
code as hinged connection will result in the corresponding internal force
component of the respective end to be released. A semi-rigid connection code
can be assigned to the in-plane rotation components of the beam ends.

Graphical symbol of a rigid connection code (the corresponding local
displacement component of the beam end is transferred to the node)

Graphical symbol of a hinged connection code (the corresponding local
displacement component of the beam end is not transferred to the node)

Graphical symbol of a semi-rigid connection code (the corresponding local
displacement component of the beam end is partially transferred to the node)
˜ Graphical symbol of a plastic connection: the maximum value of the moment
at the endpoints is calculated from the material and cross-section properties.

End releases at the
start node
End releases at the
end node

Reference point
User’s Manual 135

The table below demonstrates the use of end releases for some common cases:

F
Care must be taken not to release an element or group of elements such that rigid
body translations or rotations are introduced.
For example, if you specify spherical hinges at both ends (code: 000111), a rigid
body rotation about element axis is introduced. In this case at one of the ends
you may not release the element degree of freedom corresponding to the
rotation about local x axis (e.g. i end numerical code: 000011; j end numerical
code: 000111).
Example: Start node End node

Semi-rigid
connection
To define semi-rigid hinges set the radio button to semi-rigid and enter the
torsional stiffness of the linear elastic spring modeling the connection about
the local axis y or z. The value should be the initial stiffness of the real
connection M-φ characteristics.
The moment - relative rotation diagram of a connection is modeled by a linear
or nonlinear elastic rotational spring. The nonlinear characteristic can be used
only in a nonlinear static analysis. In a linear static, vibration, or buckling
analysis, the initial stiffness of the connection is taken into account.

Connection: Model:

Moment - Relative Rotation Diagram

136 AxisVM 8+Release 4

F
For example, in the case of steel frame structures, Eurocode 3 Annex J gives the
details of application.

Moment Resistance To fixed or semi-rigid connections a moment resistance can be assigned, that is
the maximum moment that can develop in the connection.
F
The moment resistance parameter is used only in case of a non-linear analysis.
Plastic hinge

To define plastic hinges set the radio button to plastic. Moment resistance will
be displayed but cannot be edited. If elements with different materials or cross-
sections are selected no value will appear in the edit field but hinges will be
defined with the appropriate moment resistance.
F
Plastic hinges can only be used with steel beams.

$
If any beam end release code is of a hinged connection, the beam end is
displayed on the screen as a blue circle. If it has a stiffness value a blue cross is
inscribed. If the end release corresponds to a spherical hinge, it is displayed as
a red circle.
The plastic hinges are displayed as solid circles.
The defined beams appear as dark blue lines.

Rib

Rib elements may be used, independently or in conjunction with surface
elements (plates, membranes, and shells) to model ribbed surface structures.
When used attached to surface elements, the ribs can be connected centrically
or eccentrically to the surface elements. The properties of the corresponding
surface elements are used to orient the element in the 3-dimensional space
(to define the local x-z plane).
When used independently, the ribs can model frame structures in a similar
way as the beam element, but it can take into account the shear deformations.
A reference point or vector is required to arbitrarily orient the element in the
3D space.
Rib elements are isoparametric three node, straight elements with constant or
variable (linearly changing) cross-section properties along the rib length, and
with quadratic interpolation functions. Three translational and three rotational
degrees of freedom are defined for the nodes of the element.
Three orthogonal internal forces, one axial and two shear (N
x
, V
y
, V
z
), and
three internal moments, one torsional and two flexural (T
x
, M
y
, M
z
) are
calculated at each node of each element. The variation of the internal forces
within an element can be regarded as linear.

User’s Manual 137

Define You must assign the following properties:

Material, cross-
section, local x
orientation
Defining material, cross-section and local direction X are similar to truss
elements.

Material The material of the rib can be different from the surface material
(if it is connected to a surface).

Cross-section The rib element’s cross-section is taken into account as is shown in the figure
below:

Automatic reference The reference vector will be generated by the program according to the section
References
Reference

Independent rib:
The local coordinate system is
defined as follows: the element
axis defines the x local axis; the
local z axis is defined by the
reference point or vector;
the y local axis is according to
the right-hand rule.

Rib connected to a surface element:
The local coordinate system is defined as follows: the element axis defines
the x local axis; the local z axis is parallel with the z axis of the surface
element; the y local axis is parallel with the plane of the surface element,
oriented according to the right-hand rule.
The figure below shows that when the beam is located on the edge of two
surface elements that makes an angle, the local z axis is oriented by the
average of normal axes of the surfaces. If more than two surfaces are
connected to the edge and you select one or two of them then an
automatic reference will be available when defining the rib.
The cross-sectional properties must be defined in this coordinate system.

Reference angle

The automatic local coordinate system (and the cross-section) can be rotated
around the element axis by a custom angle. If the element is parallel with the
global Z direction, the angle is relative to the global X axis. In any other case
the angle is relative to the global Z axis.

End releases End releases can be defined for ribs the same way as for beams. By default
both ends are fixed.

Eccentricity You can specify eccentricity for a rib only if it is on the edge of one or two
surfaces. If more than two surfaces are connected to the edge and you select
one or two of them you can define eccentricity for the rib.
The eccentricity (ecc) of a rib is given by the distance of the center of gravity
of its cross-section to the plane of the model of the surface (neutral plane).
It is positive if the center of gravity is on the positive direction of its local z axis.

Reference point
Reference point
138 AxisVM 8+Release 4

F
For plates, the eccentricity of the rib will modify the flexural inertia of the rib as
follows:

2 *
*exc A I I
y y
+ ·

For shells, due to the eccentric connection of the rib to the shell, axial forces will
appear in the rib and shell.

$
Ribs appear as blue lines.

Modifying Selecting elements of the same type and clicking the tool button Modifying
will be actived. Properties of elements can be changed if the checkbox before
the value is checked. If a certain property is does not have a common value its
edit field will be empty. If a value is entered it will be assigned to all selected
elements.

Pick Up>> Properties of another element can be picked up and assigned to the selected
elements. Clicking the Pick Up button closes the dialog. Clicking an element
picks up the value and shows the dialog again.
Only those properties will be copied where the checkbox is checked.

4.9.7. Surface Elements

Surface elements can be used to model membranes (membrane element), thin
and thick plates (plate element) and shells (shell element) assuming that the
displacements are small.
As surface elements you can use a six node triangular or eight/nine node
quadrilateral finite elements, formulated in an isoparametric approach.
The surface elements are flat and have constant thickness within the elements.
F
It is preferable for the element thickness not to exceed the (1/10)
th
of the smallest
characteristic size of the modeled structural element, and the deflection (w) of a
plate or shell structural element is less than 20% of its thickness (displacements
are small compared to the plate thickness).
Use of elements with the ratio of the longest to shortest element side lengths
larger than 5, or with the ratio of the longest structural element side length
to the thickness larger than 100 are not recommended
In some cases when the elements are used (that are flat with straight edges)
to approximate curved surfaces or boundaries, poor results may be obtained.

Membrane

Select the sur-
face element
type
Assign refer-
ences graphi-
cally
Assign a refer-
ence for the
local z axis
Assign a refer-
ence for the
local x axis
Reference point
Reference point
User’s Manual 139

The following parameters should be specified:
1. Plane strain or plane stress
2. Material
3. Thickness
4. Reference (point/vector/axis/plane) for local x axis
5. Reference (point/vector) for local z axis

Allows browsing of the material library to assign a material to the element.
The material selected will be added to the material table of the model.

Automatic reference:
The axis of element local directions x and z can be determined by reference
elements (see… part 4.9.17 References) or can be set automatically.

$
The center of the membrane elements is displayed on the screen in blue.

Plate

Plate elements may be used to model flat structures whose behavior is
dominated by flexural effects.

AxisVM uses an eight/nine node Heterosis finite element as plate element, that
is based on Mindlin-Reissner plate theory that allows for transverse shear
deformation effects). This element is suitable for modeling thin and thick
plates as well. Plate elements incorporate flexural (plate) behavior only
(they include no in-plane behavior).

The following parameters should be specified:
1. Material
2. Thickness
3. Reference (point/vector/axis/plane) for local x axis
4. Reference (point/vector) for local z axis

140 AxisVM 8+Release 4

Allows browsing of the material library to assign a material to the element.
The material selected will be added to the material table of the model.
Automatic reference:
The axis of element local directions x and z can be determined by reference
elements (see… part 4.9.17 References) or can be set automatically.

$
The center of the plate elements is displayed on the screen in red.

Shell

Shell elements may be used to model structures with behavior that is
dependent upon both in-plane (membrane) and flexural (plate) effects.
The shell element consists of a superimposed membrane and plate element.
The element is flat, so the membrane and plate effects are independent
(first order analysis).
F
The element can be loaded in its plane and perpendicular to its plane.
The shell internal forces are: n
x
, n
y
, and n
xy
forces (membrane components),
m
x
, m
y
, and m
xy
moments, and v
x
, v
y
shear forces (plate components).
In addition, the principal internal forces and moments n
1
, n
2
, the angle
α
n
, m
1
, m
2
, the angle α
m
and the resultant shear force vSz are calculated.
The variation of internal forces within an element can be regarded as linear.

The following parameters should be specified:
1. Material
2. Thickness
3. Reference (point/vector/axis/plane) for local x axis
4. Reference (point/vector) for local z axis

Allows browsing of the material library to assign a material to the element.
The material selected will be added to the material table of the model.

Automatic reference:
The axis of element local directions x and z can be determined by reference
elements (see… part 4.9.17 References) or can be set automatically.

$
The center of the shell elements is displayed on the screen in green.

Modifying Selecting elements of the same type Modifying will be activated. Checked
properties can be changed or picked up from another element.
Selecting elements of different types Definiton will be activated.

Pick Up>> See... Pick Up at line elements (4.9.6).

User’s Manual 141

4.9.8. Nodal Support

Nodal support elements may be used to model the point support conditions of
a structure. Nodal support elements elastically support nodes, while the
internal forces are the support reactions. Midside nodes of surface edges
cannot be supported. References are used to arbitrarily orient the x and z axes
of the element.The x axis is directed from a reference point to the attachment
node (the node to which it is attached).
You can specify the translational and/or rotational (torsional) stiffness values
about the element axes.

F
The default stiffness values are 1.000E+10 [kN/m], [kNm/rad].
$
The support elements are displayed on the screen in yellow (translational
spring) or orange (rotational spring).

F
You can define only one global support for a node. You cannot define nodal
support for a midside node of a surface element.

Reference Defines nodal support elements in the direction of a reference (point or vector).
You must select the nodes that are identically supported, and specify the
corresponding stiffness (translational Rx, and rotational Rxx).

The direction of the reference vector is
defined by the element node and its
reference point or reference vector in
the following way:

142 AxisVM 8+Release 4

Support elements oriented
toward a reference point
Support elements parallel
with a reference vector

Beam/rib relative Defines nodal support elements about
local coordinate axes of beam / rib
elements. You must select the beam /
rib elements and the nodes that are
identically supported, and specify the
corresponding translational R
x
, R
y
, R
z

If one surface is connected to the edge the local coordinate axes of the edge
are:
x = the axis of the edge
y = the axis is oriented toward inside of the surface element in its plane
z = parallel with the z local axis of the surface element

If two surfaces are connected to the edge the local z-axis direction is bisecting
the angle of surfaces. The y-axis is determined according to the right hand-rule.
If more than two surfaces are connected to the edge and you select one or two
of them then support local system will be determined based on the selected
surfaces.

Nonlinear behavior Nonlinear force-displacement characteristics can be specified for this element
as follows: compression only (very small stiffness in tension), tension only
(very small stiffness in compression). A resistance value can be also be entered.
F
The non linear parameters are taken into account only in a nonlinear analysis.
In any other case in the analysis (Linear static, Vibration I/II, Buckling) the
initial stiffnesses are taken into account.
$
Nodal supports appear as brown (R
X
, R
Y
, R
Z
) and orange (R
XX
, R
YY
, R
ZZ
) pegs in
3 orthogonal direction.

Reference point
Reference vector
Reference point
User’s Manual 143

Support stiffness
calculation

Use the Calculate... button to calculate the support stiffness (including the
rotational stiffness) due to a column type support. The support stiffnesses are
determined based on the end releases, material, and geometry of the column.

Calculating nodal support stiffness a column below and a column above the
node can be specified separately. These column parameters can also be used in
punching analysis (especially in the case of intermediate slabs). The columns
and walls modeling the supports also appear in rendered view and the cursor
can identify them.

Modifying Selecting elements of the same type Modifying will be activated. Checked
properties can be changed or picked up from another element. Selecting
elements of different types Definiton will be activated.

Pick Up>> See... Pick Up at line elements (4.9.6).
4.9.9. Line Support

Line support elements may be used to model the line support conditions of a
structure. Line support elements (Winkler type) are elastically supporting
beams, ribs, or surface edges, while the internal forces are the support
reactions. You can specify the translational and/or rotational (torsional)
stiffness values about the element axes.
Load from material
library
Load from the
cross-section library
Use the cross-section
editor
fixed/pinned at the
top of column
Fixed/pinned at the
bottom of the column
144 AxisVM 8+Release 4

The line support behaves identically in tension and compression and is
considered constant within the element.

The line support can be oriented in a direction:
Global
Beam/rib relative
Edge relative

F
The default stiffness values are 1.000E+07 [kN/m/m], or [kNm/rad/m].

F
AxisVM warns you if the condition is not satisfied (by one or more elements).
In this case the Winkler’s modulus of the defined elements are set to zero,
therefore you can divide the elements and repeat the definition/modification
process.
If you specify line supports the internal forces are linearly interpolated between
the ends of the element, therefore the division of the elements is required.

Edge relative Defines edge support elements relative to local coordinate axes of the edges.
You must specify the corresponding stiffness (translational Rx, Ry, Rz and
rotational Rxx, Ryy, Rzz).
If one surface is connected to the edge the local coordinate axes of the edge
are:
x = the axis of the edge
y = the axis is oriented toward inside of the surface element in its plane
z = parallel with the z local axis of the surface element

If two surfaces are connected to the edge the
local z-axis direction is bisecting the angle of
surfaces. The y-axis is determined according to
the right hand-rule.
If more than two surfaces are connected to the
edge and you select one or two of them then
support local system will be determined based
on the selected surfaces.

Nonlinear behavior Nonlinear force-displacement characteristics can be specified for this element
as follows: compression only (very small stiffness in tension), tension only
(very small stiffness in compression). A resistance value can aslo be entered.

F
The non linear parameters are taken into account only in a nonlinear analysis.
In any other case in the analysis (Linear static, Vibration I/II, Buckling) the
initial stiffnesses are taken into account.
$
Line supports appear as brown (R
x
, R
y
, R
z
) and orange (R
xx
, R
yy
, R
zz
) lines in
3 orthogonal direction.

Reference point
User’s Manual 145

Support stiffness
calculation

Use the Calculate... button to calculate the global or edge-relative line support
stiffness (including the rotational stiffness) due to a wall type support.
The support stiffnesses are determined based on the end releases, material,
and geometry of the wall.

4.9.10. Surface Support

Surface support Defines a surface support element (Winkler type elastic foundation) to surface
elements. You must specify a translational stiffness in the surface element local
coordinate system. The surface support behaves identically in tension and
compression and is considered constant within the element.
You must specify the support stiffness R
x
, R
y
, R
z
(Winkler’s modulus) about
the surface element local x, y, and z axes.
F
The default stiffness values are 1.000E+04 [kN/m/m], or [kNm/rad/m].

Nonlinear behavior Nonlinear force-displacement characteristics can be specified for this element
as follows: compression only (very small stiffness in tension), tension only
(very small stiffness in compression), or with resistance (the same stiffness for
compression and tension).

F
The non linear parameters are taken into account only in a nonlinear analysis.
In any other case in the analysis (Linear static, Vibration I/II, Buckling) the
initial stiffnesses are taken into account.

$
Surface supports appear as an orange square-hatched fill.

146 AxisVM 8+Release 4

4.9.11. Edge hinge

Edge hinge can be defined between domain edges or between a rib and a
domain edge. Select edge and a domain. Hinge stifness can be defined in the
local system of the edge of the selected domain.

4.9.12. Rigid elements

Rigid elements may be used to model parts with a rigid behavior relative to
other parts of the structure. Rigid elements may be used only in a linear static
analysis.
The elements can be defined by selecting the lines that connect its nodes.
The selected lines that have common nodes define the same rigid element.
There is no limit to the number of nodes of any element.
F
The degrees of freedom of the nodes of a rigid element cannot be constrained
(fixed).
Modeling membrane–beam
element connection:
Modeling eccentric beam–beam element
connection:

Define Lets you define rigid elements. You must select the lines that connect the
nodes attached to rigid elements. Recall that the lines with common nodes
define the same rigid element.

You can join or split rigid elements using the modify command.
If you select lines that connect nodes of different rigid elements, the elements
will be joined. If you deselect lines of rigid elements interrupting their
continuity, the respective elements will be split.
F
A finite element cannot have all of its lines assigned to the same rigid body.
If we want to calculate the mass of the body in a vibration analysis, place a node
to the center of gravity, connect it to the body and make this line a part of the
rigid body. Assign the mass of the body to this node.

$
The rigid elements are displayed on the screen with thick black lines.

rigid 1 2 3 rigid 1 2
User’s Manual 147

4.9.13. Spring

Spring element The spring element connects two nodes of the model. The element has its own
coordinate system. You can specify the translational and/or rotational
(torsional) stiffness values about the element axes. The element can have
nonlinear elastic stiffness properties.

The element local system can be oriented in a direction:
Global
Geometry
Reference
Element relative
Node relative

Define You must select the nodes that are connected, and specify the corresponding
stiffness (translational KX, KY, KZ and rotational KXX, KYY, KZZ). If a nonlinear
elastic spring is to be defined, you can specify resistance values, for each
internal force component.

F
Resistances will be taken into account
only in a nonlinear static analysis,
otherwise they will be ignored.

The nonlinear parameters are taken into account only in a nonlinear analysis.
In any other case in the analysis (Linear static, Vibration I/II, Buckling) the
initial stiffnesses are taken into account (that stay constant during the analysis).
148 AxisVM 8+Release 4

4.9.14. Gap

Gap element The gap element is used to model point-to-point contact. The element has two
states: one active, when it has a large stiffness value (simulates that a contact is
achieved); and one inactive, when it has a small stiffness value (simulates that
no contact is achieved). This contact model is approximate.
The gap element can be active in tension or compression. Typical force-
displacement diagrams of gaps active in tension and compression are shown
below correspondingly.

The gap element is a nonlinear element that can impose difficulties to the
solution of the nonlinear problem, due to large changes of element stiffness
when it changes status (active/inactive).
If the element is used to model regular contact problems, you may allow the
element to auto adjust its stiffness, in order to smooth the large stiffness
variations (at status changes) that can cause even divergence of the iterative
solution process.

You must specify with two nodes:

Defining local x orientation is the same as for beam elements.
Active: The active state that can be tension (a tension bolt connection) or
compression (contact of two plates)

Orientation (from one of its node to its other node)

Active stiffness: By default it is 1E+8 kN/m.

Inactive stiffness: By default it is 1E-2 kN/m.

Initial opening\penetration: By default it is 0. The initial opening can be set
based on element geometry as well (Check By Geometry). The initial opening is
a positive or zero value. While the initial opening does not close, the gap is
considered inactive.

User’s Manual 149

Auto active stiffness adjustment:
If no adjustment is selected, the values below are not taken into account.

Minimum allowed penetration: You can set a minimum value for the
penetration of the contact condition that is allowed. By default is 1E-05.

Maximum allowed penetration: You can set a maximum value for the
penetration of the contact condition that is allowed. By default is 1E-05.

Maximum adjustment ratio: If the penetration is below the minimum, the
active stiffness is softened by a maximum ratio entered here. If the penetration
is between the two limits, no action is taken. If the penetration exceeds the
allowed maximum, the active stiffness is hardened by a maximum ratio
entered here. The default value is 100. In this case, the value of the adjustment
ratio is the taken as: 1/100, 1/10, 1, 10, or 100.
F
If the gap element is used in an analysis different from a nonlinear static
analysis, the element will be taken into account as a spring with a stiffness
corresponding to its initial opening. If the initial opening is zero, the active
stiffness will be taken into account.

4.9.15. Link

Link elements Link elements connect two nodes (N-N) or two lines (L-L) and have six
stiffness components (defined in their coordinate system) that are concetrated
on an interface (located between the connected nodes/lines). Its position can be
entered relative to one node/line that is considered as reference.
Link elements can have a nonlinear parameter called limit resistance that limits
the force they are able to transfer.

Node-to-Node (N-N) Link
Connects two nodes. The stiffness components are defined in the global
coordinate system. Assigning zero value to a component the corresponding
force or moment will not be transferred from one node to the other.
The position of the interface can vary from 0 to 1 relative to the master node
(selected by the user). If the location of the interface is = 0 the interface is at
the master node. If it is = 1 the interface is at the opposite node. For any value
greater than 0 or lower than 1 the reference is between the nodes.

Example: A main girder-purlin connection (see SteelFrame.axs in the examples
folder).
Let assume that the vertical axis is Z being parallel to the local z axis. The main
girder is an IPE-400 in X-Z plane, the purlin is an I-200. You would like to
transfer forces from the purlin to the main girder but not the moments.

These elements are represented by their line of gravity. The link has to be
placed between these two axes at their point of intersection (if seen from
above). Therefore, this link has to be assigned to a vertical line having a length
equal to the distance of axes i.e. 30 cm (40/2 + 20/2). Select the node on the
main girder to be the master node of the link. The inter-face always has to be
placed at the actual point of contact. In this case the interface is located 20 cm
far (40/2) from the master node (i.e. the main girder axis). So the interface posi-
tion is 20/30 = 0.666. You assume that the connection is fixed against displace-
ments but can rotate. Therefore, you enter 1E10 for translational stiffnesses and
0 for rotational ones. If the purlins are supported only by these links you have
to enter KYY=0.001 or a similar small value to eliminate rotation around the
main girder axis.

Nonlinear
parameters
A limit resistance can be specified for each corresponding component with
non-zero stiffness.

Line-to-Line Link
Connects two lines with three nodes
each that can be rib elements and/or
edges of surface elements. A line-to-
line link has 6 nodes. The stiffness
components are defined in the local
coordinate system of the link that is in
the plane of the link element with the
x local axis parallel to the master line,
and the local z axis oriented toward
the other line in the plane of the link
and is orthogonal to the local x axis.

Assigning zero value to a component the corresponding force or moment will
not be transferred from one node to the other. The position of the interface can
vary from 0 to 1 relative to the master line (selected by the user).

If the location of the
interface is 0, the interface is
at the master line (at the
start point of the arrow).
If it is 1 the interface is at
opposite line (at the end
point of the arrow).
For any value greater than
0 or lower than 1 the
interface is between the
lines.

Let’s assume that the
vertical axis is Z, the wall is
in Y-Z plane, the floor is
parallel to the X-Y plane
and walls are represented
by shell elements. Floor
thickness is 15 cm.
You would like to transfer
forces from the floor to the
wall but not the moments.

Elements are represented by their middle plane. The wall has to reach until the
bottom plane of the floor. Links have to be placed between the upper wall
edge and the floor edge. In this case the link elements have to be in the plane
of the wall. The distance between the edges is 7.5 cm (15/2). Select wall edge
nodes to be the master nodes. The interface has to be at the actual point of
contact which is in the bottom plane of the floor and is 0 cm far from the
master node. Therefore enter 0 for the interface position. You assume that the
connection is fixed against displacements but can rotate. Therefore, you enter
1E10 for translational stiffnesses and 0 for rotational ones.

Nonlinear
parameters
A limit resistance can be specified for each corresponding component with
non-zero stiffness.

When used in conjunction with domains the following steps can be followed
to define line-to-line link elements:

1. Define the domains (See... 4.9.3
Domain) and connect the cor-
responding opposite nodes of the
domains with lines (the number of
nodes on the edges of the domains
should be equal).

2. Select the quadrilateral between the
domains. Click OK on the Selection
Toolbar.

3. Select the master line of the link
element. Click OK on the Selection
Toolbar.

4. Define the link stiffness, and set the
interface location. By default the
interface is in the midpoint of the
link element. The link element(s)
are created.

5. Now you can mesh the domains.
(See... 4.11.1.2 Mesh generation on
domain).

6. Link elements are divided
according to the domain mesh.

152 AxisVM 8+Release 4

4.9.16. Nodal DOF (Degrees of Freedom)

Lets you constrain the six nodal degrees of freedom that are:

- (translations) e
X
, e
Y
and e
Z

- (rotations) θ
X
, θ
Y
and θ
Z
.

In the default setting no nodes have constrained degrees of freedom.
In the calculations, equilibrium equations will only be written in the direction
of the free displacements (translations/rotations).
Any combination of the six nodal degrees of freedom (e
X
, e
Y
, e
Z
, θ
X
, θ
Y
and θ
Z
)
can be selected. However, in many cases typical combinations of degrees of
freedom can be used. In these situations, you can quickly apply a predefined
setting by selecting it from the list box.

Define a nodal
DOF
Use the buttons to set the degrees
of freedom. Button captions will
reflect the current value. Changes
will be applied only to those nodal
DOF which have their correspon-
ding check-box checked. Un-
checked components will retain
their original values in the selection.
You have two options to change
nodal DOF.
Overwrite
The new setting overwrites the
existing degrees of freedom
settings of the selected nodes.

Union
Performs a union set operation with the set of the new degrees of freedom
codes and the set of existing degrees of freedom codes of the selected
nodes. This option is useful in the definition of symmetry conditions.
Example of union eX eY eZ θX θY θZ
initial code: free constr. free constr. free constr.
new code: free free free constr. constr. constr.
resulting code: free constr. free constr. constr. constr.

The six nodal degrees of freedom (e
X
, e
Y
, e
Z
, θ
X
, θ
Y
and θ
Z
) are set by a six digit
code comprised of f (free) and c (constrained) symbols.
Each digit corresponds to one degree of freedom component. By default the
nodes are considered free (all digits are f-free symbols). By setting a digit to c
(constrained) the corresponding degree of freedom component is constrained.

The default DOF code of a node is [f f f f f f].

F
The loads that apply in the direction of a constrained degree of freedom are not
taken into account. Loads in the direction of the constrained degrees of freedom
will appear in the table of unbalanced loads.
$
The nodes with DOF different from [f f f f f f] are displayed on the screen in
cyan.

Degrees of freedom can be picked up from another node and assigned to the
selected nodes.

154 AxisVM 8+Release 4

4.9.17. References

Lets you define reference points, vectors or axes, and planes. The references
determine the orientation of the local coordinate systems of the finite elements
in the 3D space. The local coordinate system of the elements defined with the
references is used to define cross-sectional properties and to interpret results.
The element properties are defined and the internal forces (N
x
, V
y
, V
z
, T
x
,
M
y
, M
z
for beams, m
x
, m
y,
m
xy
for plates, n
x
, n
y
, n
xy
for membranes, etc.)
are computed in that local system.

Quick modify: Clicking on the symbol of a reference the Table Browser is
invoked displaying the table of the references. The reference vector and axis
can be defined by two points, the reference plane by three points.
When closing the table the reference vectors, and axes are normalized with
respect to 1.

$
Color codes: x = red, y = yellow, z = green.

The following references can be used:

Automatic
references
Automatic references for truss and beam elements:
A reference vector is generated and assigned to the truss and beam elements
as follows:
If the axis of the element is parallel with the global Z axis the reference
vector will be parallel to the global X axis.
In any other case it will be parallel with the global Z axis.
Automatic references for rib elements:
If the rib is independent the reference vector will be generated and assigned
to the element as for the beam elements.
If the rib is connected to a surface element, the generation of the reference
vector is as follows:
The reference vector will be parallel to the bisector of the local z axes (normal
to the surfaces) of the surfaces that have the rib element attached.
Automatic references for domains and surface elements:
Reference vectors will be generated and assigned to the surfaces as follows:
Local x-axis reference
If the plane of the surface is parallel with the X-Y plane the reference vector
for the x local axis will be generated as a vector parallel with the global X axis.
In any other case, it will be parallel with the intersection line of the surfaces
and X-Y plane.
Local z-axis reference
If the plane of the surface element is parallel to the Z axis, the generated
reference will be a vector oriented toward the origin of the global XYZ
system. In any other case it will be parallel with the global Z axis.

Reference point

Reference point is used to define the orientation (local coordinate system) of
beam, rib, support, and spring elements or to define the positive local x and z
axes of surface elements.
The reference points are defined (by its coordinates) in the global coordinate
system.

$
The reference points are displayed on the screen as small red + symbols.

User’s Manual 155

Beams, ribs, and springs:
The reference point and the element’s local x axis defines the local x-z plane.
The positive local y and z axis direction is determined by the right-hand rule.

Surface elements:
The positive local z axis is oriented toward the half-space in which the
reference point is located, and is perpendicular to the element’s plane.
Once the local x-axis is defined local y-axis is determined according to the right
hand-rule.

The local x axis will be oriented in the direction of the reference point.
In the case of a surface element the reference point must be located in the
plane of the element.

Supports:
In the case of a support element you can use a reference point to define
local x axis.

Reference vector

Lets you define the local x axis for surface, support, and spring elements.
Also defines the orientation of local z coordinate axis of beam, rib and spring
elements.

$
The reference vectors are displayed on the screen as red arrows.

Reference point Reference point
Reference point
Reference point
Reference point
Reference point
156 AxisVM 8+Release 4

Surfaces:
The local x axis will be parallel with the reference vector. In the case of a
surface element the reference vector must be parallel with the plane of the
element.
The orientation of local z-axis can also be defined by a reference vector.

Supports:
In the case of a support element you can use a reference vector to define local x
axis.

Beams, ribs, and springs:
The reference vector and the element’s local x axis defines the local x-z plane.
The positive local y and z axis direction is determined by the right-hand rule.

Reference Axis

Reference axis is used to define the local x-axis of surface elements, that will be
oriented towards the reference axis. The reference axis must not include
element centerpoint.

$
The reference axises are displayed on the screen as red arrows.

Reference vector Reference vector
User’s Manual 157

Reference Plane

Reference plane is used to define the local x axis of surface elements, that will
be parallel to the intersection line of the reference plane and the plane of the
element. The reference plane must not be parallel with the plane of the
element.

Reference angle

Rotation of truss / beam / rib cross-sections is made easy by the reference angle.
The automatic local coordinate system (and the cross-section) can be rotated
around the element axis by a custom angle. If the element is parallel with the
global Z direction, the angle is relative to the global X axis. In any other case
the angle is relative to the global Z axis.

$
The reference plane is displayed on the screen as a red triangle.

4.9.18. Creating model framework from an architectural model

This icon starts the conversion operation of the architectural model
if previously an ArchiCAD interface file (*.ACH) or an IFC file (*.IFC)
was loaded by File / Import (See... 3.1.6 Import.) as a background layer.

Display Select architectural project stories and element types you want to be displayed.
F
Use the built-in Filter to enhance selection.

If you create model framework or delete objects and nothing is selected the
Selection Toolbar appears. Click the Property Filter icon to select beams and
columns within a certain range of section size according to their minimum side
length or select walls or slabs within a certain range of thickness.
If you want to restore the whole range click the button at left bottom.
If the Only objects without static model is checked only elements not having static
model will be selected.

F
Deleting an architectural object having a static model will not delete its
associated static model.

158 AxisVM 8+Release 4

Create Model
Framework
Model framework will be created from selected layer elements. Columns will
be reduced to their axis, walls, slabs and roofs will be reduced to their center
plane. Framework nodes and lines become part of the AxisVM model and are
independent of the background layer.
Parts will automatically be created for levels and object types and the elements
created for the static model will be included in the appropriate parts.
Hinged wall connections can be modeled using edge hinges when creating
a model framework from the architectural model.

You can assign properties to the selected architectural objects as follows:

Slab

Floors can be defined as
plates or shells. Assign a
material and a thickness.
For layered floors, the
thickness of the layers will
appear in the layer list.
You can select the layers that
you want to take into
account.

Wall

Walls can be defined as
membranes or shells. Assign
a material and a thickness.
For layered walls you can
choose to apply the thickness
of the load bearing layer, the
total thickness or a custom
value.
Apply bottom support:
You can automatically assign
a support to the bottom edge
of the selected walls.

Convert walls to supports: You can convert wall objects to supports by
enabling this checkbox. The support will be placed at the top edge of the
corresponding wall. The support stiffness will be computed based on the top
and bottom end releases.

Load from Material
Library
User’s Manual 159

Column

Column objects are always
converted to beam elements.
Assign a material and a cross-
section. If Auto is selected
the cross-section is created
based on the geometrical
description of the architec-
tural object.
You can assign a support to
the bottom of the column.

Convert columns to supports: The selected column objects can be converted to
supports. The support stiffness is established based on the end releases.
The supports will be placed at the top of the column.

Beam

Beam objects are always
converted to beam elements.
Assign a material and the
cross-section.
If Auto is selected the cross-
section is created based on
the geometrical description
of the architectural object.

Roof

Roof objects are always
converted to shell elements.
Assign a material and a cross-
section.
For layered roofs, the
thickness of layers will
appear in the layer list.
You can select the layers that
you want to take into
account.

4.9.19. Modify
Lets you modify the definition of the selected elements.
1. Holding the [Shift] key down, select the elements to modify. You can
use the Selection icon as well.
2. Click the element’s icon on the Elements Toolbar.
3. In the element’s dialog window check the properties you want to
modify. Property fields show the common value in selection. If selected
elements have different values the field is empty.
4. Modify the respective properties as desired.
5. Click the OK button to apply the modifications and exit the dialog
window.
F
In fact, the modification is similar to the element definition, but does not assign
properties to undefined geometrical elements and allows access to a specific
property without altering others. You can switch to the element definition radio
button to define all properties of all the selected elements, lines or surfaces.
Immediate mode If the Geometry or Elements tab is active click a finite element to modify its
properties. If more finite elements have been selected they can be immediately
modified by clicking one of them. If you click an element which is not selected,
selection disappears and you can modify the element you clicked. If you click
on a node its nodal degrees of freedom can be edited immediately.
You can also modify the properties using of Property Editor.
See... 3.5.1 Property Editor

4.9.20. Delete
[Del] See... 3.2.5 Delete

4.10. Loads

Lets you apply various static loads for static and buckling analysis, and define
concentrated masses for vibration analysis.

User’s Manual 161

4.10.1. Load Cases, Load Groups
Load Case

Lets you set the current, create new, and modify or delete existing load cases.
Any load you create will be stored in the current load case. In the professional
version the number of load cases is not limited. In the standard version a
maximum of 99 cases can be created. Load groups can also be created from the
different load cases.

Load Case Lets you set the current, create new, and modify or delete existing load cases.
Any load you create will be stored in the current load case. In the professional
version the number of load cases is not limited. In the standard version a
maximum of 99 cases can be created. Load groups can also be created from the
different load cases.
New Case You must assign a different name to each case. The following are the three
types of load cases that you can choose from when you want to create a new
case:

1. Static
The static load case can be applied to static, vibration, and buckling
analysis. In case of vibration analysis, the loads can also be taken into
account as masses.
The load case can be included into a load group. When calculating the
critical load combination, the load case will be taken into account
according to the parameters of the load group to which it belongs.
F
Critical combination can be determined only from the results of a linear static
analysis.
2. Influence line
Lets you apply a relative displacement load to obtain the influence line of
a result component, of a truss or beam element.
F
When the influence line load case type is selected you can apply only the
influence line load ->
162 AxisVM 8+Release 4

3. Seismic
When selecting seismic load case type you can specify the parameters for
calculation of earthquake loads. Prior to creating an seismic load case, you
must perform a vibration analysis. Based on the mode shapes, and on the
structural masses, AxisVM generates seismic loads case, in a k+2 number,
where k is the number of available smallest frequencies. The two
additional cases corresponds to the signs +, and -, that contain the critical
combinations. See... 4.10.20 Seismic Loads

F
In case of selecting seismic load case only the Seismic parameters icon will be
available ->
4. Tensioning
If tensioning calculation according to the current design code is supported,
tensioning load cases can be created. These load cases always get into a ten-
sioning load group. After defining a load case with the name name, two load
cases will be created. name-T0 will contain the equivalent load calculated for
the end of tensioning process, name-TI will contain long term values of the
equivalent load. Any of these load cases can be selected to define tension-
ing. After definition just loads for name-T0 will be calculated as static analy-
sis results are required to determine the long term equivalent loads.
See details… 4.10.21 Tensioning
Duplicate Lets you make a copy of the selected load case under another name. You must
specify the new name, and a factor that will multiply the loads while copying.
The factor can be a negative number as well.
F
Selected loads can be copied or moved to another load case by changing load case
during the copy or move process.

Delete Lets you delete the selected load case.
You can change the current load current case by
selecting from the drop down list near the load case
icon.
F The name of the selected load case will appear in the
Info window and the loads you define will get to this
load case.

In case of choosing Tensioning load case only the
Tensioning Icon will be active on the toolbar.
Click on it then select the proper beam or rib
elements, so the Tensioning Dialog will appear.
See... 4.10.21 Tensioning

Click right mouse button over the list, select Order of load cases to get to a
dialog setting the load case order. This dialog is also available in the Table
Browser (Format / Order of load cases).

Order of load cases... Display order of load cases can be set by the following options.

Move selected case to the top.

Move up selected case.

Move down selected case.

Move selected case to the end.

Sort by alphabetical order

Sort by load groups

Follow creation order

User’s Manual 163

Load group You can select the load group you want to place the current load case in from
the dropdown list. Load case will immediately be moved to its new position in
the tree view. You can also drag and drop load cases between load groups by
mouse.

Setting the current load case :
Click on any existing load cases from the list which is on the left side of the
Load Groups & Load Cases dialog window. The chosen load case will
become the current case. Any subsequently defined loads will belong to
the newly selected load case.

Safety Class Select the safety class of the building from the combo box. Changing the safety
class may require changes in the incidental group factors γ
f;q
, Ψ and Ψ
t
.

Load Group Load groups are used when generating of critical (design) values of the results.

New Group Lets you define a new load group. You must specify the name and the type
(permanent, incidental, exceptional) of the load group, and the corresponding
factors according to the current design code. Later you can specify which load
cases belong to a specific load group.
Clicking any icon within the New Group group box will create a new group in
the tree and you can specify a name for it. Existing load group names will be
rejected. After creating a load group you have to specify the value of its
paremeters (like the safety factor, dynamic factor, simultaneity factor, etc.).
A load case can be assigned to a load group by choosing a group from the
dropdown list or dragging the load case under a load group in the tree.

See... 4.10.2 Load Combination

The following load groups are allowed depending on the design code:
1. Permanent
Includes dead load, permanent features on the structure...
Include all load cases in combinations
All load cases from the group will be taken into account in all load combi-
nations with their upper or lower safety factor.
Include the most unfavourable load case only
Only the most unfavourable load case will be taken into account from the
load group with its upper or lower safety factor.

2. Incidental
Includes live load, wind load, snow load, crane runway load...
Can be simultaneous with exceptional goups
If checked load case(s) from the group can act together with a load case
from an exceptional group in critical combinations.
Simultaneous load cases
Any number of load cases from the group can act simultaneously in
critical combinations.
Mutually exclusive load cases
In a critical load combination only one load case from the group will be
taken into account at one time.

3. Exceptional
Includes earthquake, support settlements, explosion, collision... Only one
load case from the group will be taken into account in a load combination
at one time. That load case must have the simultaneity factor of 0 · α .

164 AxisVM 8+Release 4

4. Seismic load group (Eurocode, SIA 26x, DIN 1045-1, STAS and
Italian code)
Only one load case from the group will be taken into account in a load
combination at one time. That load case must have the simultaneity factor
of 0 · α .

5. Tensioning load group (if tensioning can be calculated according to the
current design code)
Tensioning load group is handled as a permanent load group. It can contain
only tensioning load cases. Both load cases for the same tensioning (name-T0
and name-TI) cannot be included in any load combination.

Lets you define load combinations of the defined load cases. You can specify a
factor for each load case in a load combination. The results of a load
combination will be computed as a linear combination of the load cases taking
into account the specified load case factors. A zero factor means that the
respective load case does not participate in the load combination.

Inserts a load combination table to the current report.

Calculates all critical combinations based on load groups and transfers them
into the load combination table.

F
You can also define load combinations after you have completed a linear static
analysis. Then, when required the postprocessor computes the results of these
load combinations.
In case of nonlinear static analysis, AxisVM first generates the combination case,
and then performs the analysis (a load combination at a time).

User’s Manual 165

Automatic load
combination
The program builds all possible combinations depending on the load groups
parameters and the equations of the current design code.
The minimum and maximum result values of these combinations are selected
as critical (design) values.

Critical load combination method for internal forces and for displacements are
selected automatically. Critical load combination method for displacements
depends on the type of structure you are modeling. Click Result Display
Parameters on the Static Toolbar then click Select. If your current design code
is Eurocode you can set the critical combination formula at the bottom of the
dialog.

Lets you apply forces/moments to the selected nodes.
You must specify the values of the load components
F
X
, F
Y
, F
Z
and M
X
, M
Y
, M
Z
, in the global coordinate
system.
If you apply a nodal load to a node that is already
loaded, you can overwrite or add it to the existing
load.

The positive directions are according to the positive directions of global
coordinate axes.

Modify nodal loads You can select, move, copy or modify the load independently of the node.

Modify position 1. Select the loads you want to move together.
2. Grab any of them by pressing the left mouse button.
3. Move them to their new position.
4. Click the left mouse button or use a command button. (Enter or Space).

Nodal loads can be moved onto a beam, a rib or a domain.
Signs of the load values are calculated according to the right hand rule.

F
Load components applied in the direction of a constrained degree of freedom will
be not taken into account in the analysis.
$
The forces are displayed on the screen as yellow arrows, the moments as green
double arrows.

User’s Manual 167

4.10.4. Concentrated Load on Beam

Lets you apply concentrated forces/moments to the selected beam finite
elements. You must specify the values of the load components FX, FY, FZ,
MX, MY, MZ in the local or global coordinate system.
If you apply a concentrated load to a node that is already loaded, you can
overwrite or add it to the existing load.
Concentrated loads can be selected, moved, copied, modified independently of
the beam. Modify load values like in case of nodal loads.
The positive directions are in accord with the positive directions of the local or
global coordinate axes.

$
The forces are displayed on the screen as yellow arrows, the moments as green
double arrows.

4.10.5. Point Load on Domain

Applies a point (concentrated) load at the location of the cursor if it is over a
domain. You can also enter the location of the load by its coordinates. You can
place loads by clicking the left mouse button or pressing any of the command
buttons. See... 4.7.2 Entering Coordinates Numerically

The direction of the load can be:
- Global (with respect to the global coordinate system)
- Local (with respect to the local (element) coordinate system)
- Reference (with respect to a reference)

168 AxisVM 8+Release 4

Modify point load
on domain
You can modify the location and value (intensity) of the load:

Modify position 1. Select the load with the cursor (a load symbol appears beside the
cursor).
2. Keep left mouse button depressed.
3. Move the mouse or enter the relative coordinates to move the load to a
new location.
4. Release left mouse button to set the load in its new location.

Modify value 1. Select the load with the cursor.
2. Click the left mouse button.
3. Enter the new load values in the dialog.
4. Click on the Modify button to apply the changes and close the window.

If the load is projective, the value of the load that is applied to the beam/rib is
α sin ⋅ p , where α is the angle of the load direction and the beam/rib axis.
F
For rib elements you can apply line loads distributing along the entire length of
the rib only.

4.10.7. Edge Load

170 AxisVM 8+Release 4

Lets you apply distributed (constant) loads to the selected edges of the selected
surface elements.
If more than two finite elements are connected to the edge or they have
different local coordinate systems you have to select both the edge and the
finite element when you specify the local load. Load will be defined in the
local system of the selected element.

In the case of shell elements, the load that is applied in global coordinate
directions can have a projective distribution. If the load p is projective, the value
of the load that is applied to the shell is p cos α , where α is the angle of the load
direction and the element plane normal.
User’s Manual 171

4.10.8. Domain Line Load

Applies a uniform or linear distributed line load over a domain.
The direction of the load can be global projective, global along element or local.
The m
x
is always the torsional moment (around the application line of the
load). Set load components and placement method then draw the load
(or click the lines) to place it.

Line load between
two points

Line load along a
polyline

Distributed line load
on an existing line
or arc

Click any line or arc on the domain boundary or within the domain to apply
the load previously defined. This type of load is associative.
Moving the boundary or the internal line moves the load as well. Deleting the
line deletes the load.

Modify of the load You can modify the location and value (intensity) and any vertex of the load
polyline:

Modify location 1. Select the load with the cursor.
2. Keep left mouse button depressed.
3. Move the mouse or enter the relative coordinates to move the load to a
new location.
4. Release left mouse button to set the load in its new location.

Modify shape 1. Move the cursor above the vertex (a load polyline vertex symbol
appears beside the cursor).
2. Click the left mouse button
3. Drag the vertex to its new position after pressing the left mouse button.
4. Click the left mouse button.

Modify value 1. Select the load with the cursor (a load symbol appears beside the
cursor).
2. Click the left mouse button.
3. Enter new load values in the dialogue window.
4. Click on the Modify button to apply the changes and close the window.

The domain element type determines the load type and direction as follows.
For a membrane domain the load must be in the plane of the domain.
For a plate domain the load must be perpendicular to the plane of the domain.
For a shell domain any load direction is acceptable.
The load can be a global load on surface, a global projective load or a local load
and the components will be interpreted accordingly.
You can select between constant or linear load intensities and set if loads
disapper over holes or are distributed on the edge of the hole.

Loads disappear/
allowed on holes
The first icon represents the option that loads over holes are not applied to the
structure. The second one represents the option that loads over holes are
distributed on the edge of the hole.

Constant load
Steps of load definition in case of constant load:

Rectangular area
load

1. Enter load components (p
x
, p
y
, p
z
)
2. Enter two diagonal end points of the rectangle by clicking or by coordinates.
(This function is available only on the X-Y, Y-Z and X-Z planes)

Polygon load
1. Enter load components (p
x
, p
y
, p
z
)
2. Enter polygon vertices by clicking or by coordinates. In this latter case press
an extra Enter after specifying the last position. If you enter the polygon
by clicking on the domain close the polygon by clicking on the first vertex
again or by double-clicking at the last vertex. Instead of the left mouse
button you can also use Space or Enter key to enter polygon vertices.

The load will be distributed over the domain. The shape of this type of load
will automatically follow any change in the domain geometry. Within a load
case you can apply only one load of this type on a domain. New distributed
domain load definition always overwrites the previous one.

174 AxisVM 8+Release 4

Linear load
Steps of load definition in case of linear load:

The plane of the load intensity can be specified by load intensity values
(p
1
, p
2
, p
3
) at three points [(1), (2), (3)] in the plane of the domain. These points
are the load value reference points. If you want to use the same reference
points and values to many loads of different shape and position you can lock
the reference points and values by clicking the Lock button. Loads are applied
by entering an area.

Define load value reference points

Lock/unlock value reference points

Rectangle area load
1. Enter load values at the reference points (p
1
, p
2
, p
3
).
2. Enter two diagonal end points of the rectangle by clicking or by coordinates.
(This function is available only on the X-Y, Y-Z and X-Z planes)
3. Enter three reference points by clicking or by coordinates.

Skewed rectangle
area load
1. Enter load values at the reference points (p
1
, p
2
, p
3
).
2. Enter three corners of the rectangle by clicking or by coordinates.
3. Enter three reference points by clicking or by coordinates.

Polygon load
1. Enter load values at the reference points (p
1
, p
2
, p
3
).
2. Enter polygon vertices by clicking or by coordinates. In this latter case press
an extra Enter after specifying the last position. If you enter the polygon
by clicking on the domain close the polygon by clicking on the first vertex
again or by double-clicking at the last vertex. Instead of the left mouse
button you can also use Space or Enter key to enter polygon vertices.
3. Enter three reference points by clicking or by coordinates.

Within a load case you can apply only one load of this type on a domain.
New distributed domain load definition always overwrites the previous one.

Modify area load The position, shape and intensity of a mesh-independent area load can be
changed.

Modify position 1. Place the mouse above the load contour (the cursor will identify the load).
2. Press the left mouse button and move the mouse.
3. Find the new load position by moving the mouse or by coordinates.
4. Drop the load by clicking the left mouse button or pressing the Space or
Enter key.

Modify shape 1. Place the mouse above a vertex of the load polygon (the cursor will identify
the load polygon vertex as a corner).
2. Press the left mouse button and move the mouse.
3. Find the new vertex position by moving the mouse or by coordinates.
4. Place the vertex by clicking the left mouse button or pressing the Space or
Enter key.The load shape will change.

Modify intensity 1. Place the mouse above the load contour (the cursor will identify the load).
2. Click the left mouse button. The area load windows appears.
3. Change the load intensity values.
4. Click on the Modify button to confirm the changes.

User’s Manual 175

Multiple loads can be selected and modified this way.

Area load intensity and shape can also be changed in the Table Browser
by changing the appropriate values in the load table.

Delete Select the loads to delete and press [Del]

F
Mesh-independent loads are not affected by removing or re-creating a meshes on
domains.

4.10.11. Surface load distributed over beams and ribs

A constant surface load can be distributed over beams and ribs. It is useful
when modelling snow or wind load on beam structures.
1. Click the icon and select the load distribution range in the dialog.

Auto distributes the load over the elements
under the load. Any new beam or rib defined
under the load will redistribute the load.

To selected elements only distributes the load
over the selected elements only. Select lines
using the selection toolbar. Distribution re-
mains the same if a new beam or rib is de-
fined under the load.

2. Define load polygon the same way as for a constant domain area load.

The load polygon can be a rectangle,
a skewed rectangle or any closed
polygon. The fourth method on the
icon tollbar is to click lines of a closed
beam/rib polygon. This way the load
becomes associative. Moving the ele-
ments or their end nodes changes the
load polygon accordingly.

176 AxisVM 8+Release 4

4.10.12. Fluid Load

Lets you apply pressure
loads characteristic to fluids
to the selected plate or shell
elements. The actual load is
calculated from values
computed at the corner of
the elements.

Fluid loads created with the same definition will be handled as one load.
So if you specified a fluid load on more than one element and click on the load
contour on any of these elements the load will be selected on all of them and
you can easily change the load parameters.
To change a fluid load only on certain elements use partial selection, i.e. draw
a selection frame around the elements.

4.10.13. Dead Load

Lets you take the dead load of the elements (that have materials assigned) and
domains into account in the analysis. The dead load is computed based on the
cross-sectional, the mass density of the material, the gravitational acceleration
g, and the length or area of the element. The load is applied as a distributed
load in the direction of the gravitation vector.

$
A dashed line is drawn along line elements or surface/domain contours.
If load intensity labels are turned on a light blue G appears.

4.10.14. Fault in Length (Fabrication Error)

This load type is used when a structural beam element is shorter or longer
than required due to a fault in manufacturing.
Lets you apply the load, which is required to force the shorter/longer beams to
fit the distance of the corresponding nodes, to the selected elements.
You must specify the value of the manufacturing fault, dL [m]. A positive dL
means that the beam is longer by dL.
The load has the same effect as the ( ) dT dL L
·
· ⋅ α thermal load.

User’s Manual 177

4.10.15. Tension/Compression

Lets you define an initial axial internal force in truss/beam elements.
The load has the same effect as a ( ) dT P E A
·
· − ⋅ ⋅ α thermal load.

4.10.16. Thermal Load on Line Elements

Lets you apply temperature loads to the selected line elements
(truss, beam, and/or rib).
You must specify values for the following parameters:

dT= T - Tref is the temperature variation that is taken into account in the
analysis. A positive dT means a warm up of the truss.

Beam/Rib Tref: - reference temperature (corresponding to the initial unstressed state)
T
1
: - the temperature of the top cord (in the corresponding local direction)
T2: - the temperature of the bottom cord (in the corresponding local direction)

dT
=
=T - Tref is the uniform temperature variation that is taken into account in
the analysis, where T is the temperature of the cross-section in its center of
gravity.

in local y direction:
y
G
H
y
T T T T ) (
2 1 2
− + ·

in local z direction:
z
G
H
z
T T T T ) (
2 1 2
− + ·

where,
yG, zG, and Hy, Hz are properties of the cross-section.
A positive dT
=
indicates a temperature increase of the beam.

dT
#
=T1 - T2 is the non-uniform temperature variation that is taken into
account in the analysis.

178 AxisVM 8+Release 4

4.10.17. Thermal Load on Surface Elements

Lets you apply temperature loads to the selected surface elements.
You must specify values for the following parameters:

Tref: - reference temperature (corresponding to the initial unstressed state)
T1: - the temperature of the top cord (in the positive local z direction)
T2: - the temperature of the bottom cord (in the negative local z direction)

dT
=
=T - Tref is the uniform temperature variation that is taken into account in
the analysis, where T is the temperature in the center of gravity of the cross-
section.

dT
#
=T1 - T2 is the non-uniform temperature variation that is taken into
account in the analysis.

F
For membranes only dT
=
is taken into account.
For plates only dT
#
is taken into account.

4.10.18. Forced Support Displacement

Lets you apply forced displacements to the selected support elements.
You must specify the values of the forced displacement components
(translational: e [m]; rotational: θ [rad]).
AxisVM approximates the problem, by applying a force P
support
in the direction
of the support element so as to produce the forced displacement e.

T
2

T
1

Reference point
User’s Manual 179

e K P
port port
⋅ ·
sup sup

where
K
support
is the corresponding support stiffness.

If the stiffness of the support element is large enough, the secondary
deflections due to other loads will be negligible. Therefore, you may apply
forced displacements only to the supports stiff enough relative to the stiffness
of the structure (at least 10
3
times larger) in the corresponding direction.
Check this assumption every time, by checking the displacement results and
verifying the displacement at the respective node.
A positive forced displacement moves the node in the positive direction of the
local axis.

4.10.19. Influence Line

Lets you apply a relative displacement load to obtain the influence line of an
internal force component, on the selected truss/beam elements.
You must specify the value of the relative displacement e as +1 or -1.
F
You can define influence line load, only in an influence line type load case.
See...4.10.1 Load Cases, Load Groups
Truss
You can specify the value of the relative displacement e
x
as +1 or -1.

The seismic loads are taken into account
according to the Response Spectrum
Analysis method. This method requires a
previously calculated number of un-
damped free vibration frequencies and the
corresponding mode shapes.

Based on these vibration mode shapes AxisVM generates equivalent static
loads (for each vibration mode shape) which are then applied to the model in a
static analysis. Then internal force results obtained for each mode shape are
summed using to the method described in design code specifications.
Seismic analysis can be performed based on the following design codes:
• Eurocode 8 (EN 1998-1:2004) • DIN (4149:2005-04)
• Swiss code (SIA261:2003) • Romanian code (P 100-92)
Design codes
• Italian code (OPCM 3274) • Hungarian (MI-04.133-81)

The program performs only the analysis described below. Any other sup-
plementary analysis required by the design codes must be completed by the
user. AxisVM can calculate extra torsional moments due to random eccentri-
cities of masses and check the sensitivity of stories to second order effects.
Seismic load
generation, setting
parameters
These are the steps of creating seismic loads and setting response spectrum
parameters:
1. Calculate the first n vibration mode shapes and frequencies.
Check the table of seismic equivalence coefficients in X, Y, Z directions in the
Table Browser. Vibration results will appear only if you call Table Browser
from the Vibration tab page.

F
Each design code requires that the mode shapes must represent a certain ratio of
the total mass. E.g. In Eurocode 8 the requirement is • • 0.9 (the sum of the
coefficients must represent at least 90% in each direction) and every mode shape
having a coefficient larger that 5% in any direction must be included.
User’s Manual 181

2. Create a new seismic load case.
The program will create multiple load cases:

a.) Without extra torsional effects:
Load cases with endings X, Y and Z. The result of these cases will contain
the maximum displacements and forces summed up from seismic effects in
X, Y or Z direction.
Load cases with endings + and –. The results of these cases will contain the
positive and negative maximum displacements and forces summed up
from seismic effects in X, Y and Z direction.

b.) With extra torsional effects:
Load case with endings Xa, Xb, Ya, Yb. The results of these load cases will
contain the maximum forces and displacements calculated from the seismic
effect in X or Y direction and the torsional effect with a + eccentricity (Xa
and Ya) or with a – eccentricity (Xb and Yb).
Load case with ending Z. The results of this load case will contain the
maximum forces and displacements calculated from the seismic effect in Z
direction.
Load cases with endings 1+ and 1-. The results of these load cases will
contain the maximum forces and displacements calculated from the sum of
Xa, Ya and Z with a + or – sign.
Load cases with endings 2+ and 2-. The results of these load cases will
contain the maximum forces and displacements calculated from the sum of
Xa, Yb and Z with a + or – sign.
Load cases with endings 3+ and 3-. The results of these load cases will
contain the maximum forces and displacements calculated from the sum of
Xb, Ya and Z with a + or – sign.
Load cases with endings 4+ and 4-. The results of these load cases will
contain the maximum forces and displacements calculated from the sum of
Xb, Yb and Z with a + or – sign.

Select any of these cases.

F
The effect of seismic forces in Z direction will be taken into account only if a
vertical response spectrum is defined.

3. Setting seismic parameters

Clicking this button you can set the response spectrum and other parameters.

The program uses two different spectra for the horizontal and vertical seismic
effects.
You can create a spectrum in two ways
1. Define a custom spectrum.
2. Define a parametrical spectrum based on Eurocode 8
EC8 EN1998-1 (4.2.4.)

F
The above parameters can be changed when defining the parametric spectrum.
a
g
: design ground acceleration
• : lower limit for the horizontal design spectrum (the recommended value
is 0.2).
q : behaviour factor for horizontal seismic effects. It depends on the type and
material of the structure. This factor connects the linear analysis results
and the nonlinear (elastic-plastic) behaviour of the structure.

Torsional effects (optional) EC8 EN 1998-1 (4.3.3.3.3.)
AxisVM calculates extra torsional forces around a vertical axis due to random
eccentricities of masses for every story and modal shape using the maximum
X and Y sizes of stories:

Extra torsional moments due to seismic effects in X or Y direction are

) 05 . 0 (
Yi Xi tXi
H F M ⋅ t ⋅ ·
) 05 . 0 (
Xi Yi tYi
H F M ⋅ t ⋅ ·
where
F
Xi
and F
Yi
are the horizontal forces belonging to a modal shape of the ith story
due to seismic effects in X or Y direction. Torsional moments will be taken into
account with both (+ and –) signs but always with the same sign on all stories.

Calculating displacements
Displacements coming from nonlinear behaviour are calculated this way:
E q E
d s
⋅ ·
where
q
d
: behaviour factor for the displacements
E : maximum displacement form the linear analysis
F
Usually q
d
=q.
Check of second order seismic sensitivity EC8 EN 1998-1 (4.4.2.2.)
At the end of a seismic analysis AxisVM checks the second order seismic
sensitivity of each story. The sensitivity factor ƒ is calculated from the seismic
effects in X or Y direction:

User’s Manual 185

h V
d P
tot
r tot
⋅
⋅
· θ

where,
P
tot
is the total gravitational load above and on the story
d
r
is the interstory displacement calculated from the differences of average
displacements between stories with a seismic effect in X or Y direction.
V
tot
is the total seismic shear force above and on the story coming from a
seismic effect in X or Y direction.
h is the interstory height

Seismic parameters
(Eurocode 8)

Seismic parameters, response spectra and combination methods can be set in a
dialog.

Spectral function
editor

Setting the Design spectrum type combo from Parametric to Custom and
clicking on the Spectral Function Editor icon a dialog appears. Spectrum can be
created/modified as a function consisting of linear segments. Segment points
listed on the left hand side can be edited.

Combination of modal responses
It is possible to let the program choose the combination method of modal
responses by turning on the Automatic radio button. If T
j
/ T
i
< 0.9 is true for all
vibration mode shapes (i.e. the modal responses can be considered to be
independent) then the program choose SRSS method. In other cases the
CQC method will be chosen.

Combinations of the components of seismic action
The quadratic formula or the 30%-method can be chosen.

AxisVM uses two spectra for the analysis: one for horizontal seismic effects and
one for vertical ones.
A design response spectrum can be defined as a user-defined diagram or in a
parametric form based on SIA 261:2003 (16.2.4.)

where
a
gd
: horizontal design ground acceleration
ƒ
f
: importance factor of the building
q : behaviour factor for horizontal seismic effects which depends on the type
and material of the structure. q is the link between the linear calculation
and the nonlinear (elastic-plastic) behaviour of the structure.
S, T
B
, T
C
, T
D
: the default values of these parameters depend on the soil class
based on SIA 261:2003 (Table 25)

The vertical parametric design response spectrum is based on the horizontal
one. a
gd
and q must be replaced by a
gdv
and q
v
,
where
a
gdv
: vertical design ground acceleration, (a
gdv
= 0,7a
gd
)
q
v
: behaviour factor for vertical seismic effects

Torsional effects (optional) SIA 261:2003 (16.5.3.4.)
AxisVM calculates extra torsional forces around a vertical axis due to random
eccentricities of masses for every story and modal shape using the maximum
X and Y sizes of stories:

Extra torsional moments due to seismic effects in X or Y direction are
) 05 . 0 (
Yi Xi tXi
H F M ⋅ t ⋅ ·
) 05 . 0 (
Xi Yi tYi
H F M ⋅ t ⋅ ·
where
F
Xi
and F
Yi
are the horizontal forces belonging to a modal shape of the ith story
due to seismic effects in X or Y direction. Torsional moments will be taken into
account with both (+ and –) signs but always with the same sign on all stories.

Check of second order seismic sensitivity EC8 EN 1998-1 (4.4.2.2.)
At the end of a seismic analysis AxisVM checks the second order seismic
sensitivity of each story. The sensitivity factor ƒ is calculated from the seismic
effects in X or Y direction:

User’s Manual 189

h V
d P
tot
r tot
⋅
⋅
· θ

where
P
tot
is the total gravitational load above and on the story
d
r
is the interstory displacement calculated from the differences of average
displacements between stories with a seismic effect in X or Y direction.
V
tot
is the total seismic shear force above and on the story coming from a
seismic effect in X or Y direction.
h is the interstory height

Seismic parameters
(SIA 261:2003)

Seismic parameters, response spectra and combination methods can be set in a
dialog.

Spectral function
editor

Setting the Design spectrum type combo from Parametric to Custom and
clicking on the Spectral Function Editor icon a dialog appears. Spectrum can be
created/modified as a function consisting of linear segments. Segment points
listed on the left hand side can be edited.

Combination of modal responses
It is possible to let the program choose the combination method of modal
responses by turning on the Automatic radio button. If T
j
/ T
i
< 0.9 is true for all
vibration mode shapes (i.e. the modal responses can be considered to be
independent) then the program choose SRSS method. In other cases the
CQC method will be chosen.

Combinations of the components of seismic action
The quadratic formula or the 30%-method can be chosen.

4.10.20.3. Seismic calculation based on Italian Code
Italian code

Design response spectrum
S
d
(T) for linear analysis
AxisVM uses two spectra for the analysis: one for horizontal seismic effects and
one for vertical ones.
A design response spectrum can be defined as a user-defined diagram or in a
parametric form based on the Italian code.
Parametric design response spectrum for horizontal seismic effects:
S
d

a
g
: design ground acceleration
q : behaviour factor for horizontal seismic effects. It depends on the type and
material of the structure. This factor connects the linear analysis results and
the nonlinear (elastic-plastic) behaviour of the structure.

Seismic parameters, response spectra and combination methods can be set in a
dialog.

Spectral function
editor

Setting the Design spectrum type combo from Parametric to Custom and
clicking on the Spectral Function Editor icon a dialog appears. Spectrum can be
created/modified as a function consisting of linear segments. Segment points
listed on the left hand side can be edited.

Combination of modal responses
It is possible to let the program choose the combination method of modal
responses by turning on the Automatic radio button. If T
j
/ T
i
< 0.9 is true for all
vibration mode shapes (i.e. the modal responses can be considered to be
independent) then the program choose SRSS method. In other cases the
CQC method will be chosen.

Combinations of the components of seismic action
The quadratic formula or the 30%-method can be chosen.

Combination of spatial components
Resultant maximum displacement and force values can be calculated from the
coexisting effects in X and Y direction:

2 2
Y X
E E E + ·
where
E
X
and E
Y
are the maximum values of independent seismic effects in
X and Y direction.
F
The resultant forces are always positive. When creating a seismic load case two
different cases will be created with an ending of + and –. In the first case forces
will be positive, in the second case negative. These load cases can be used to build
combinations and determine critical load combination.

where
E
X
and E
Y
are the maximum values of independent seismic effects in
X and Y direction.
F
The resultant forces are always positive. When creating a seismic load case two
different cases will be created with an ending of + and –. In the first case forces
will be positive, in the second case negative. These load cases can be used to build
combinations and determine critical load combination.

Seismic parameters
(Romanian Code)

where
Τ
c
: corner period
V
e
: velocity of the seismic wave
L
c
: the biggest horizontal size of the structure
A warning message is sent if following inequality is not satisfied:
3
1
<
⋅
r e
c
T V
L

F
If a warning message is displayed, the results of the analysis are inaccurate, and
in general lead to over-dimensioning.

196 AxisVM 8+Release 4

4.10.21. Tensioning

Prestressing
(Post tensioning)
Tendons can be assigned to a continuous selection of beam or rib elements.
After defining tendon properties and the tensioning process AxisVM deter-
mines the immediate losses of prestress and the equivalent loads for the end
of tensioning (load case name-T0). After completing a static analysis it deter-
mines the time dependent losses of prestress and the long term equivalent
loads from the result of quasi-permanent combinations (load case name-TI).
Tendon trajectory tables can be generated with user-defined steps.

Tendons The first tab is to define tendon parameters and geometry.

Icons on the vertical toolbar beside the tendon list are

Add new tendon. Geometry for the new tendon can be defined using the toolbar
beside the diagram.

Geometrical tansformations of tendons

Tendons selected in the tree can be translated or mirrored. Tendons can be
copied or just moved. Copied tendons inherit the original parameters and the
tensioning process assigned to them.

Delete tendon. Deletes the selected tendon.

User’s Manual 197

Parameters of the selected tendon appear beside the tendon list. Parameter
values can be edited.

unintentional angular displacement for internal tendons per unit
length. Shows the precision of workmanship.
Ususally 0,005 < k < 0,01.
R
min
Minimum radius of curvature. Where the radius of curvature is
smaller than this limit tendons are displayed in red.

To draw tendon geometry click the icons on the vertical toolbar beside the
drawing and enter base points. AxisVM determines the trajectory passing
through these base points as a cubic spline to minimize curvature. For each
basepoint the angles of tangent can be specified by setting the α (top view) and
β (side view) values in the table. Enter values between -180° and 180°. Initial
values are 0°. Existing base points can be dragged to a new position using the
mouse.

Draw tendon in 2D. Base points can be created by clicking the diagram or using
the coordinate window. Double-click or Mouse Right Button/Complete to make
the base point the last one. The tendon position within the cross-section has to
be specified only at the first base point. Further base points will be in the local
x-z plane containing the first base point.

Steps of drawing a tendon in 2D:
1. Select the postion of the cross-section where you want to define the
tendom basepoint.
Settle the tendon onto the proper position in the cross-section view.
You can position the tendon onto the top or at the bottom of the
cross-section considering the concrete cover.

Position the tendon onto an optional point

Position the tendon onto the neutral axis

Position the tendon onto the top of the cross-section

Position the tendon onto the bottom of the cross-section

2. Following the first location you can position the other points of the
tendon onto the longitudinal section.

Draw tendon in 3D. The tendon position within the cross-section has to be
specified at every basepoint. You can close a tendon geometry with using
Mouse Right Button/Complete.

Steps of drawing a tendon in 3D:
1. Select the postion of the cross-section where you want to define the
tendom basepoint.
2. Settle the tendon onto the proper position in the cross-section view.
Following the first location repeat the step 1. and step 2. to define all base-
point.

Add new base point. Click the cable to add a new base point. In case of several
tendons this function only works with the active tendon.

Delete base point. Clicking an existing base point deletes it. After deleting the
second base point the tendon geometry is deleted. In case of several tendons
this function only works with the active tendon.

198 AxisVM 8+Release 4

Table of base points Base point properties can be edited in the table. Use the toolbar beside the ta-
ble to add base points or remove the selected lines.

Options. Grid and cursor settings of the longitudinal and the cross-section dia-
gram can be set. See… 2.15.14.1 Grid and Cursor

Tensioning pro-
cess
The second tab is to define the tensioning process for tendons by determining
the order of certain operations.

Possible operations and parameters:

Tensioning from left / right /
both side

Release from left / right / both
side
Force as a fraction of the characteristic value
of tendon steel tensile strength (f
pk
).

Anchor on left / right / both side Wedge draw-in of the anchorage device

Deletes the last operation from the list.

Concrete The third tab is to check the material
properties of the concrete. e
cs
(∞) is
the long term value of the concrete
shrinkage strain. Its value can be en-
tered here.

User’s Manual 199

Results If valid parameters, geometry and tensioning process is assigned to every ten-
don, result diagrams are displayed on the fourth tab. If one tendon is selected
in the tree two diagrams are shown. The first one is the actual tension along
the tendon (f
p
/f
pk
), and the equivalent load for the tendon (F). If more than one
tendon is selected the diagram shows the resultant equivalent load for the se-
lected tendons only.

Immediate losses of tension
1. Tension loss due to friction between tendons and their ducts (sleeves) at po-
sition x measured from the anchorage point along the tendon is calculated as
) 1 ( ) (
) (
max
kx
e x
+ Θ µ −
µ
− σ · σ
,
where
σ
max
is the maximum tension in the tendon
Θ

is the sum of the absolute angular displacements over a distance x

2. Losses due to the instantaneous deformation of concrete are calculated as
∑
]
]
]

σ ∆
· ∆
cm
c
p p el
E
j
E A P ,
where
∆σ
c
is the variation of stress at the centre of gravity of the cross-section
j = (n–1) / 2n, where n is the number of stressing steps
E
cm
is the secant modulus of elasticity of concrete

3. Losses at anchorage are due to wedge draw-in of the anchorage devices.

where ρ
1000
= 2,5% is the relaxation loss at a mean temperature
of 20°C at 1000 hours after tensioning
ϕ final value of creep coefficient
σ
c,QP
is the stress in the concrete adjacent to the tendons, due to self-
weight and initial prestress and other quasi-permanent actions
where relevant.
A
p
is the total cross-section area of tendons
A
c
is the cross-section area of the concrete
I
c
is the second moment area of the concrete section
z
cp
is the distance between the centre of gravity of the concrete sec-
tion and the tendons

Trajectory table The last tab is to build a trajectory table for the selected tendons with the de-
sired increment and optional shift of origin. The trajectory table consists of the
local y and z coordinates of the selected tendons at the calculated x positions.
The defined basepoints are always displayed in the Trajectory Table.

Main toolbar The main toolbar has two buttons.

Copy diagram
Ctrl+C
Copies the drawing on the active tab to the Clipboard as a Windows metafile.
This way the diagram can be pasted to other applications (e.g. Word).

User’s Manual 201

Print
Ctrl+P
Prints a report of the tensioning using diagrams and tables. Tendons and re-
port items can be selected. You can choose the position of the drawing
(landscape or portrait) and set the scale of it (Print options for drawings).

Cross-sections can be selected to print cross-section diagrams.

Menu You can reach the following functions via the menu:

File

Print See... Main toolbar / Print

Edit

Undo/Redo Undoes the effect of the previous command./ Executes the command which
was undone.

Join connecting
tendons
If more than one beam or rib element has been selected and these elements
contain connecting tendons this function joins the connecting tendons.
The joining works in case of single element, too.

202 AxisVM 8+Release 4

Window

Coordinates Editing of the longitudinal and cross-section diagrams is made easier by a co-
ordinate window. The display of this window can be turned on and off.

Status On diagrams an information window appears displaying diagram-specific in-
formation. The display of this window can be turned on and off.

4.10.22. Nodal Mass

In a vibration analysis the masses are concentrated at nodes that you can take
into account by their global components MX, MY, MZ .
In second-order vibration analysis, the loads due to the nodal masses are
applied on the model, as well as the masses due to the applied loads.
If mass is the same in each direction it is enough to specify one value after
checking Apply the same mass in each direction..

$
The nodal mass is displayed on the screen as two dark red concentric circles.

4.10.23. Modify
Modify To modify loads:
1. Press the [Shift] key and select loads you want to modify (or the loaded
elements). You can also select by drawing a selection frame or using the
Selection Toolbar.
2. Click the load type icon on the Toolbar.
3. Check the checkboxes beside the values you want to change.
4. Enter new values.
5. Close the dialog with OK.

Immediate mode If the Loads tab is active click a finite element to modify its loads.
If the element has more than one load only one of them will come up.
If you have placed different concentrated and distributive loads on a beam and
click the beam the load nearest to the click position will come up.
If more finite elements have been selected their loads can immediately be
modified by clicking one of them. If you click an element which is not selected,
selection disappears and you can modify the element load you clicked.

F
In fact, load modification is similar to the load definition, but does not assign
loads to elements not being loaded and allows access to a specific load property
without altering others. You can switch to the Define radio button to place loads
on all the selected elements, lines or surfaces.

If we select elements with loads not matching the load type we choose these loads
remain unchanged.

User’s Manual 203

4.10.24. Delete
[Del] See... 3.2.5 Delete

4.11. Mesh

Clicking the mesh tab mesh toolbar becomes available with mesh generation
for line elements and domains, mesh refinement functions and a finite element
shape checking.

4.11.1. Mesh Generation

Automatic detection of overlapping lines and missing intersections during
meshing reduces the errors in model geometry.

4.11.1.1. Meshing of line elements

Finite element analysis uses linear elements with constant cross-section
so arced and variable cross-section (tapered) line elements must be divided
into parts. This is called line element meshing. The accuracy of the solution
depens on the mesh density.
This mesh can be removed or modified just like a domain mesh. Removing a
mesh does not delete loads and properties assigned to the line element.
A mesh can also be defined for linear elements with constant cross-section.
It is useful in nonlinear or vibration analysis when it is required to divide line
elements to achieve a higher accuracy.

Mesh parameters
for line elements

Mesh generation can be performed according to different criteria:
Maximum deviation from arc
Chord height cannot exceed the value specified.
Maximum element size
Length of the mesh lines cannot exceed the value specified.
Division into N segments
Line elements are divided into N parts.
By angle
Central angle of arced mesh segments cannot exceed the value specified.

204 AxisVM 8+Release 4

4.11.1.2. Mesh generation on domain

A mesh of triangular surface elements can be generated on the selected
domains by specifying an average surface element side length for the mesh.
Meshing will take into account all the holes, internal lines and points of the
domain. Meshes can also follow loads above a certain intensity.

Meshing
paramaters for
domains

Mesh size An average mesh element size can be specified. The actual mesh can contain
smaller and larger elements as well.

Contour division
method
Uniform mesh size
Domain boundaries and inner lines will be divided according to the mesh
size to ensure the given element size.
Adaptive mesh size
Adaptive meshing follows domain geometry and refine the mesh by
reducing element size wherever it is necessary.

If Create mesh only for unmeshed domains is checked no mesh will be created
for domains already meshed.

The progress of the mesh generation process can be monitored in a window,
and can be canceled any time with the Abort button.

The mesh generator uses only the end-points of beam elements that are in the
plane of the domain, and disregards their corresponding line segments.
Rib elements are incorporated with their line segments because they can be
defined on surface edges as well.

If there are existing quadrilateral or triangular meshes within the domain,
the mesh generator will not change these meshes, and will integrate them in
the new mesh.

Before Meshing After Meshing

F
If a mesh is generated over an existing domain mesh (with a different average
element side length), the new mesh will replace the existing one.
User’s Manual 205

4.11.2. Mesh Refinement

Lets you refine the finite element mesh of surfaces. The elements in the refined
mesh have the same properties (material, cross-section / thickness, references,
etc.) as those in the coarse mesh.
F
You have to manually set the nodal degrees of freedom of the newly generated
mesh that were not set automatically during the process of mesh generation.
The following options are available:

Uniform

Lets you refine the entire selected mesh. You must specify the maximum side
length of a surface element in the refined mesh.

Before mesh refinement

After mesh refinement

Bisection

Lets you refine the selected mesh by bisecting the elements as shown in the
figure below

Quadrilateral element

Triangular element

Node relative

Lets you refine the mesh around the selected nodes (locally around columns,
nodal supports). You must specify a division ratio (0.2-0.8). The command
refines the mesh dividing the elements connected to the respective nodes
by the defined ratio.

Before mesh refinement After mesh refinement
206 AxisVM 8+Release 4

Lets you refine the mesh around the selected nodes (locally around columns,
nodal supports). You must specify a division ratio (0.2-0.8). The command
refines the mesh dividing the elements connected to the respective nodes
by the defined ratio.

Edge relative

Before mesh refinement After mesh refinement

Lets you refine the mesh along the selected edges (locally along edge
supports/loads). You must specify a division ratio (0.2-0.8). The command
refines the mesh dividing the elements connected to the respective edges
by the defined ratio.

4.11.3. Checking finite elements

Program checks the minimum angle of surface finite elements (α).

A triangular finite element is distorted if • 15.
A qudrilateral finite element is distorted if • 30.

User’s Manual 207

5. Analysis
AxisVM lets you perform static, vibration and buckling analysis. It implements
an object-oriented architecture for the Finite Element Method.
The instructions included in this User’s Manual assume a preliminary
knowledge of the finite element method and experience in modeling.
Note that the finite element analysis is only a tool, not a replacement for
engineering judgment.

The actual running times of each step, and details of the model can be
displayed by pressing the Details button.

Model verification The input data is verified in the first step. If an Error is found a warning
message is displayed and you can then decide whether to cancel or continue
the analysis. Then, a node numbering optimization is performed in an iterative
form to reduce the half-bandwidth of the system stiffness matrix.
The node renumbering has effect only during the analysis process, the results
are displayed in the original node numbering. Press Esc key to skip this
sequence.

Performing the
analysis
AxisVM displays the evolution of the solution process by two progress bars.
The bar on the top displays the current step performed, while the other
displays the overall progress of the analysis process.

The equilibrium equations in the direction of constrained degrees of freedom
are not included in the system of equations. Therefore to obtain support
reactions you must model the support conditions using support elements.

The Cholesky method is applied to the solution of linear equilibrium
equations. The eigenvalue problems are solved with the Subspace Iteration
method.
208 AxisVM 8+Release 4

Error of the solution Solution error is calculated from the solution of a load case with a known
result. It is a good estimation of the order of errors in displacement results for
other load cases.
Info palette shows this error as E(EQ).
If the value of E (Eq) is greater than 1E-06 the reliability of the computed
results is questionable. It is expected, that the Error of the displacements is of
the same order.

Result file
generation
During the processing of the results the program sorts the results according to
the original order of the nodes and prepares them to graphical display.

In the following chapters we ‘ll show the setting of the parameters of the each
calculation methods.

5.1. Static Analysis
The term static means that the load does not vary or the variation with the time
can be safely ignored.

Linear static

Performs a linear static analysis. The term linear means that the computed
response (displacement, internal force) is linearly related to the applied load.
All the load cases are solved in the analysis. Through the geometric linearity,
it is assumed that the displacements remain within the limits of the small
displacement theory. Through the material linearity, it is assumed that all
materials and stiffness characteristics are linear-elastic. The materials assigned
to surface elements can be othotropic.
F
See the description of the gap, and spring elements in Chapter 4, on how to use
these elements in a linear analysis.

Nonlinear static

Performs a nonlinear-elastic static analysis. The term nonlinear means that the
computed response (displacement, internal force) is nonlinearly related
to the applied load. This can be due to the use of gap, link or non-linear
support, truss or spring elements, or taking into account the geometric
nonlinearity of truss, beam, rib and shell elements.

User’s Manual 209

Select load cases or combinations in the tree view. AxisVM will perform
nonlinear analysis for the selected load cases and shows a progress dialog.

Solution control
Force
When the Force control is selected, the increments are applied as equal
fractions of the loads (as one parameter load).
Displacement
When displacement control is selected, the increments are applied
as equal fractions of the displacement component of the node specified.
Load factor
Load factor can be used to multiply loads of the selected load case
or combination for the nonlinear analysis.

Number of increments
Lets you specify the number of increments. The default value is 1.
When highly nonlinear behavior is analyzed, you may specify a greater
value in order to achieve convergence.

Convergence criteria
Based on the convergence tolerances you specify, AxisVM will determine
if the nonlinear solution has reached the required accuracy (convergence).
Therefore it is important that the convergence tolerances to be set
properly. During the iteration process, the norm of the unequilibrated
load and/or of the iterational displacement increment vector must vanish
(to approach zero).

Maximum iterations
You can set the maximum number of the iterations based on the
specifics of your model, and of the incremental solution parameters.
By default the value is set to 20. If the convergence is not achieved
within the maximum number of iterations, no results will be obtained.
Displacement/Load/Work/Convergence criteria
In case of a nonlinear calculation you can specify multiple criteria,
in terms of load, displacement, and work, for monitoring the
convergence of the nonlinear solution. At least one criteria has to be
selected. The criteria expressed in terms of work can be adequate for
most problems. However, you may encounter a small Error in your
unequilibrated load while the Error in displacements is still large, or
vice-versa.
Factors of convergence criteria has the following default values: 0.001
for displacements, 0.001 for force, and 0.000001 for work.
The relative errors at the end of the iteration process appear in the info
window.
E(U): relative error of the displacement convergence
E(P): relative error of the force convergence
E(W): relative error of the work convergence
210 AxisVM 8+Release 4

Use reinforcement in calculation

When analyzing reinforced concrete plates it is possible to take the
calculated or actual reinforcement into account.
Displacements and internal forces of reinforced concrete plates are
calculated according to the moment-curvature diagram of the reinforced
cross-section of the plate. These results show the actual plate deflection
and forces in the plate.
Include geometric nonlinearity

The equilibrium is established with respect to the deformed line elements.
Geometric nonlinearity can be taken into account only for truss, beam, rib
and shell elements. If your model does not include nonlinear finite
elements (gaps, springs, supports, and/or links), this check-box is
automatically enabled. If nonlinear elements are included in the model,
by enabling this check-box, you may or may not include the geometrical
nonlinearity for the above mentioned line elements (truss, beam, rib
and shell).

F
The beam elements must be divided in at least four parts when geometric
nonlinearity is taken into account.
Store last increment only

Allows you to reduce the size of the results file when an incremental
nonlinear analysis is performed with multiple increments (load
or displacement) when just the results of the last increment are of interest
to you. You can enable this checkbox when you do not need the results of
previous increments.

F
You should disable this check-box if you want to trace the load-displacement or
other (nonlinear) response of the structure.

AxisVM applies a Newton-Raphson iteration technique to the iterational solution
of each increment. The technique is known in different variants, depending on the
update of the system (stiffness) matrix.
The following example shows the behavior of a one degree of freedom spring
system with load control:

If n=1 (default), the system stiffness
matrix is updated in each iteration.
The method is known as the classical
Newton-Raphson technique.
If n > MaxIterations, the system
stiffness matrix is updated only once,
in the first iteration of each increment.
The method is known as the Modified
Newton-Raphson technique.

User’s Manual 211

If 1<n<MaxIterations, a
variant of the Modified
Newton-Raphson technique
is obtained. In the figure
above the iterative process is
shown for the case n=2.

F
The stiffening systems, usually lead to more significant numerical solution
problems (than the softening systems), and solutions with n>1 can lead to
divergence. This is why, when gap elements change their state (from active to
inactive or vice-versa), a system stiffness matrix update is triggered, even though
it would not be required based on the value specified for n.

The softening systems, and the so-called snap-through phenomenon cannot be
analyzed with load controlled increments. You must apply a displacement
control to pass through the peak points.

Displacement
control
This figure shows a load control applied
to a nonlinear system. The incremental
solution fails in the 5
th
increment.
To find the peak value of the load-
displacement characteristics of the sys-
tem, you must apply a displacement
control technique.

5.2. Vibration

F
Lets you determine the lowest
natural frequencies and mode
shapes corresponding to the
free vibration of an undamped
linear structure when no exter-
nally applied loads are com-
puted. AxisVM verifys whether
the required number of the
lowest eigenvalues has been de-
termined.
The system mass matrix has a
diagonal structure and includes
only translational mass com-
ponents.
The solution technique applied to
the associated generalized eigen-
value problem is designed to find
the lowest real and positive
eigenvalues. It is not suitable to
find eigenvalues that are zero or
nearly zero.

212 AxisVM 8+Release 4

Solution control

Lets you specify the parameters of the incremental solution process:
First-order
The solution does not include the effect of axial forces of truss/beam
elements on the system stiffness.
Second-order
The solution include the effect of axial forces of truss/beam elements
on the system stiffness.
Tension axial forces have a stiffening effect, while the compression
axial forces have a softening effect. These effects influence the free
vibrations of the structure.
Case
Lets you select a case. The loads are converted into masses.
If a second-order analysis is selected, the results of a linear (first-
order) static analysis, that precedes the vibration analysis, will be
accounted too.
Number of mode shapes
Lets you specify the number of the vibration mode shapes you want
to evaluate. A maximum number of 99 can be requested. The default
value is 6. The value specified here can not be larger than the number
of the system’s mass degrees of freedom.
Convert loads to masses
You can enable the conversion of the gravitational loads into masses,
and take these concentrated masses into account.
Masses only
You can analyze models without loads, but with masses, and take
element masses into account.
Include mass components
Only checked mass components will be used in the analysis.
It is useful when calculating modal shapes only in a certain direction.

Convergence criteria

Based on the convergence tolerances you specify, AxisVM will determine
if the calculated eigenvalues and eigenvectors have the required accuracy.
Therefore it is important that the convergence tolerances be set properly.
Maximum number of iterations
You can set the maximum number of the iterations based on the
specifics of your model, and the number of eigenvalues requested
(more iterations for more eigenvalues). By default the value is
set to 20. If the convergence is not achieved within the maximum
number of iterations, no results will be obtained.
Eigenvalue convergence
Lets you specify the convergence tolerance for the eigenvalues.
The default value is 1.0E-10.
Eigenvector convergence
Lets you specify the convergence tolerance for the eigenvectors.
The default value is 1.0E-5.
F
Due to the lumped mass modeling technique to achieve the required accuracy the
elements must be divided into more elements (by refining the mesh).
Usually at least four finite elements must correspond to each half wave.
A good rule-of-thumb is that beams must be divided into at least eight elements.
The mode shapes are normalized with respect to the mass:

{ ¦ [ ] { ¦ 1 · ⋅ ⋅ U M U
T

User’s Manual 213

5.3. Buckling

Lets you determine the
lowest (initial) buckling load
multipliers and the corres-
ponding mode shapes.
AxisVM verifys whether the
required number of the
lowest eigenvalues has been
determined. The buckling
load multiplier n
cr cr
· λ is
computed, solving the
eigenvalue problem. λ
cr
is
the smallest eigenvalue and
the corresponding eigen-
vector is the buckling mode
shape.

The Sturm sequence check is applied to verify whether the computed eigen-
values are the lowest. 0 <
cr
λ means that buckling occurs for the opposite load
orientation and
cr
effectiv
cr
λ λ ≥ .
F
The solution technique applied to the associated generalized eigenvalue problem
is designed to find the lowest real and positive eigenvalues. It is not suitable to
find eigenvalues that are zero or nearly zero.

Solution control

Lets you specify the parameters of the incremental solution process:
Case
Lets you select a case that will be taken into account. A linear
(first-order) static analysis, that precedes the buckling analysis, will be
performed.
Number of mode shapes
Lets you specify the number of the vibration mode shapes you want
to evaluate. A maximum number of 99 can be requested. The default
value is 6. The lowest positive eigenvalue is of main importance.

Convergence criteria
See... 5.2 Vibration/Convergence criteria

Beams/ribs The buckling of beams/ribs is considered as in-plane buckling
(flexural buckling), which means that the deformed shape of the element
remains in a plane and the cross-section does not warp.
For buckling analysis the beam cross-section must be defined by specifying
its principal moments of inertia.
F
The beam elements must be divided into at least four elements.

Trusses The flexural buckling of truss elements are not considered by the program.
You must calculate the buckling load of each truss manually, or by modeling
the trusses by four beam elements with the corresponding end releases.

If 0 >
cr
λ the instability is caused by loads in the reverse direction and the
critical load parameterfor the given case is
cr
efectiv
cr
λ λ ≥

If the model contains trusses the critical load parameter of global structural
buckling will be computed only. Buckling of individual trusses is not analysed.

214 AxisVM 8+Release 4

5.4. Finite Elements
All finite elements may be used in a linear static or first-order vibration, and
buckling analysis. (Note that not all elements have geometric stiffness.)
Geometrically nonlinear static and second-order vibration analysis can be per-
formed only on frame structures.

5.5. Main Steps of an Analysis
1. Define the geometry of the structure, the material and cross-sectional
properties of the members, the support conditions, and the loads.
2. Determine the load transfer path.
3. Determine local discontinuities such as stiffeners, gussets, holes.
4. Determine the type of finite elements that will best model the behavior
of the structure. With this step the properties of structural elements will
be concetraded in their neutral axis (point, axis, or, plane).
5. Determine a mesh type and size for the model. The size of the mesh
have to correspond to the desired accuracy of the results and with the
available hardware.
6. Create the model:
a.) Equivalent geometry
b.) Equivalent properties
c.) Topology of the elements
d.) Equivalent support conditions
e.) Equivalent load (static) or masses (vibration, response-spectrum)
7. Check input data (accuracy, compatibility)
8. Run analysis
9. Select important results
10. Evaluate and check the results
a.) Accuracy and convergence of the solution
b.) Compatibility taking into account point 6.d.
c.) Uncommon structures shall be analyzed with other methods and/or
software as well.
11. Restart analysis with a correspondingly updated model, if in step 10
a criteria is not satisfied.
12. Evaluate the results by the means of isoline/isosurface plots, animation,
tables... Draw conclusions on the structure’s behavior.
Modelling To build a model of a structure you have to accept many assumptions so you
also have to keep the effects of these assumptions in view when evaluating
results.
The finite element method provides an approximative solution for surface
models. To make the model match the real solution you have to use finite
element meshes with an appropriate density. Making finite element meshes
you have to take into account the expected stress distribution, the model
geometry and the materials, supports and loads used.
The position af nodes and mesh lines (called the topology of the finite element
mesh) depends on the geometrical discontinuities (irregular contours,
line supports) and the discontinuities of loads (concentrated loads, terraced
load values for line loads).
At stress concentration points (sharp corners) you have to refine the mesh.
To avoid singularities due to concentrated effects you can distribute them on a
small area around the point of effect.
Arc contours can be approximated as polygons. Using very small tolerance in
this approximation leads to polygons with extreme small sides. The very dense
mesh created on this contour may cause the model exceed the capacity of your
computer.
In general if you refine the mesh you get more precise results.

The determinant of the stiffness matrix is zero or negative due to modeling
error.

Singular Jacobian matrix

Determinant of the element’s Jacobian matrix is zero, due to distorted
element geometry.

Excessive element distortion during deformation

The element has been excessively distorted in the current increment.

Too large rotation increment

The rotation increment of an element exceeds π/4 radian (90°). You should
increase the number of load increments.

Invalid conrol displacement component

The displacement control is applied about a constrained degree of
freedom.

Convergence not achieved

The number of iteration is too low.

Too many eigenvalues

The rank of the mass matrix is lower than number of requested
eigenvalues (frequencies or buckling modes).

No convergent eigenvalue

No eigenvalue converged.

Not the lowest eigenvalue (xx)

There are xx lower eigenvalues than the lowest the one determined

Element is too distorted

The geometry of the finite element is distorted. In order to maintain the
accuracy of the results you should modify the finite element mesh to avoid
too distorted element geometries.

Excessive Element Deformation

During a nonlinear analysis excessive deformations developed the
element within an increment (load or displacement). You should increase
the number of increments.

No convergence achieved within maximum number of iterations

There was no convergence within the maximum number of iterations
(see... Static Analysis/Nonlinear Static Analysis/Solution Control para-
meters). You can increase the number of iteration. The model may not
converge at the respective load level, and you should change the Solution
Control parameters accordingly.

Divergence in the current iteration

A divergence was detected in the iteration process. Increments are too
large or the convergence criteria are too loose.

No stiffness at node ... in direction ...

There is a singularity in the system stiffness matrix corresponding to that
degree of freedom. You should check the support and degrees of freedom
(DOF) settings of your model.

218 AxisVM 8+Release 4

This page is intentionally left blank.

User’s Manual 219

6. The Postprocessor
Static Lets you display the results of a static analysis. (6.1)
Vibration Lets you display the results of a vibration analysis. (6.2)
Buckling Lets you display the results of a buckling analysis. (6.3)
R.C. Design Lets you display the results of a reinforced concrete design analysis. (6.4)
Steel Design Lets you display the results of a steel design analysis. (6.5)

6.1. Static
The Static menu item allows you to display the tools for displaying and
interpreting the static analysis results.

Start a linear static
analysis
See...5.1 Static Analysis

Start a nonlinear
static analysis
See...5.1 Static Analysis

Result display
parameters
Lets you set the options of the graphical display of the results.
You can select the results of a load case/combination or critical load
combination.

Depending on the performed analysis you can select the results of a linear
or nonlinear static analysis. Each analysis type can be further defined:
Case
Lets you display the results of any load case/combination.
Envelope
Lets you display the envelope of the results from the selected load cases
and/or load combinations. The program searches for the minimum
and/or maximum values at each location of the selected result component.
Critical
Lets you generate the critical load combinations, according to the load
group definitions, for each location of the selected result component.

Display Values

If you selected envelope or critical you can choose from the following options:

Min+Max
Displays the minimum and maximum values of the current result
component.
Min
Displays the minimum (sign dependent) values of the current result
component.
Max
Displays the maximum (sign dependent) values of the current result
component.

Investigate all
combinations
resulting in the
same maximum
value
By default this option is off. AxisVM takes into account combinations resulting
in an extreme for any result component. In certain design methods however a
combination which produces no extremes can be more unfavorable.
In this case turn this option on. In design calculations AxisVM will build all
possible combinations and check them according to the design code require-
ments. As the number of combinations can be extremely high this option is
recommended only if the model size and the number of load cases are small.

Method of
Combination
If Critical combination formula is set to Auto
AxisVM determines if ULS (ultimate limit
state) or SLS (service limit state) combination
is required based on the result component.
If Critical combination formula is set to Custom
Min / Max / Min, Max results of all combina-
tion methods will be available in the load
case combo tree regardless the current result
component.
In case of Eurocode, DIN 1045-1, SIA 262
and other Eurocode based design codes the
formula for creating SLS combinations can
be chosen.

Display Mode Diagram
Lets you display the current result component in a colored diagram form.
The numerical values are displayed if a Show Value Labels On option
is enabled.
Section line
Lets you display the current result component in the active section lines
and/or planes in a diagram form. The numerical values are displayed
if the Show Value Labels On option is enabled.
Isoline (contour line)
Lets you display the current result component in a line color contour plot
form. The values that are represented by the isolines are specified in the
Color Legend window. You can set the parameters of the Color Legend
window as was described in the Information Windows paragraph.
The numerical values are displayed if a Show Value Labels On option is
enabled.
Isosurface 2D or 3D
Lets you display the current result component in a filled color contour
plot form. The ranges that are represented by the isosurfaces are specified
in the Color Legend window. You can set the parameters of the Color
Legend window as was described in Information Windows paragraph.
The numerical values are displayed if a a Show Value Labels On option is
enabled. See...2.17.3 Color Legend Window
None
The current result component is not displayed.
Section lines Lets you set the active section lines, planes and segments. If display mode is set
to Section line result diagrams will be drawn only on active (checked) section
lines. Symbol of the section planes can be displayed enabling the Draw section
plane contour checkbox. Turning on the Draw diagram in the plane of elements
option changes the appearance of all section diagrams.
To change this parameter individually use the Section lines dialog.
See... 2.15.11 Sections

Component Lets you select the result component to be displayed.

Scale by Lets you set the scale of a diagram drawing. The default value is 1, when the
maximum ordinate is represented as 50 pixels.

Write Values to ... Nodes
Writes the values of the current result component to the nodes.
Lines
Writes the values (intermediate values if applicable) of the current result
component to the line elements.
All surfaces
Writes the values of the current result component to the surface elements.
The maximum absolute value of the nine values computed at the nodes of
each surface is displayed, and the respective node is marked by a small
black circle.

222 AxisVM 8+Release 4

Min/max only
Writes the local min/max values only of the current result component
to the nodes, lines and surfaces.

m
y
moment component R
z
support force component

After clicking the Miscellaneous Settings... button the following options
are available:

Result Smoothing
Parameters
None
The values of the internal forces of the surface elements computed at
the nodes are not averaged.
Selective
The values of the internal force components of the surface elements
computed at the nodes are averaged in a selective way, depending on
the local coordinate systems, the support conditions and the loads of
the elements that are attached to a node.

All
The values of all internal force components of the surface elements computed
at the nodes are averaged.
Intensity Reference
Value
Lets you display the variation of the current internal force component within
the surface elements in a filled color contour plot form. The numerical values
are displayed if a Show Value Labels On option is enabled.
See... 6.1.8 Surface Elements Internal Forces

F
If Min,Max envelope or critical load combination is selected,
the Isoline and Isosurface 2D cannot be selected.

Display scaling
factor

Lets you scale the display of the diagrams.

6.1.1. Minimum and Maximum Values

Lets you search the minimum and
maximum value of the current result
component. If you are working on
parts, the search will be limited to the
active parts.
AxisVM will mark all occurrences of the
minimum / maximum value.

F
If parts are displayed extreme values are
determined from the displayed parts
only.

224 AxisVM 8+Release 4

6.1.2. Animation

Lets you display the displacements, internal forces, and mode shapes in
animated form (frame by frame). The animation consists of a sequence of
frames that are generated by linear interpolation between initial values
(frame 0) and the actual values of the current result component (frame n),
according to the number of frames (n).

Unidirectional play
Plays the frames starting from
frame zero and ending with
frame n.
Animation

Bi-directional play
Plays the frames starting from
frame zero and ending with
frame n and then the reverse.

Recording Options Frames
Lets you set the number of animationframes. You must specify a value
between 3 and 99. More frames produce smoother but slower animation.
Rendered
Each frame consists of a rendered display.

Colored
Each frame consists of an iso-line/surface display. The colors are animated
according to the color legend.

Video File You can create a video file, name.avi.
Click Save button to save the parameters of the video file.

You can set the duration of displaying a frame. Lower duration will result in a
bigger number of frames. A number of 30 frames/second is usual, therefore you
should not normally enter less than 30 ms for the duration of a frame.

Lets you display the X-Y diagram of any two nonlinear analysis result
components. Two diagrams can be displayed at a time.
You have to select the result components for each diagram. In addition to the
regular result components, you can assign the load parameter or the increment
number to any axes (X or Y).

Display parameters settings of Diagrams:

6.1.4. Result Tables

Table Browser lets you display the numerical values of the results in a table in
customizable form. If you switched on parts, the table will list the values
corresponding to the active parts. If you selected elements the table will list the
selected elements only by default. You can change the range of listed elements
by clicking the property filter button on the Table Browser toolbar.
You can transfer data to other applications via Clipboard.
See... 2.9 Table Browser.
Diagram parameters
226 AxisVM 8+Release 4

Displaying results
[Ctrl]+[R]
After calling the Table Browser you can set if you need a detailed table and/or
the extremes and you can select which components you need the extremes
from. This dialog can be called later from Format / Result Display Options.
Results Unchecking this option removes the
detailed results leaving the extremes
as the only content of the table.

Extremes Unchecking this option removes the
summary of extremes from the end
of the table.

Extremes to find You can set the components for which you want to find the extreme (maximum
and minimum) values. Among the minimum and maximum values the
concomitant values of the different result components are displayed if the
minimum/maximum values occur in a single location or otherwise.
If there are multiple locations the symbol * will appear, and in the Loc
(location) column the first occurrence of the extreme value will be displayed.

When you display the results of critical combinations in addition to the minimum
and maximum values, the load cases that lead to the critical values
are included with the following notations:
[ ... ] represents the results of a permanent load case.
{ ... } represents the results of an incidental load case.
( ... ) represents the results of an exceptional load case.

6.1.5. Displacements
Node
At each node, six nodal displacement
components (three translations and three
rotations) are obtained in the global
coordinate system.
The resultant values of translations (eR) and
of rotations (θR) are also determined.

Displaying the displacements of a cantilever (membrane model):

Diagram with nodal values Section line with nodal values

Isolines Isosurfaces 2D

Beam For each beam element the intermediate displacements are obtained in the
local and global coordinate systems. When displaying the displacements of the
structure the beam displacements are related to the global coordinate system.
If you pick the cursor on a beam element the six beam displacement
components related to the element local coordinate system are displayed in a
diagram form.
You can display displacements of more than one beam element if:
a) The local coordinate system of the elements are almost or entirely
identical. See... 2.15.14.3 Drawing/ Contour line angle
b) The local x orientation is the same.
c) The elements have the same material

228 AxisVM 8+Release 4

You can display the diagrams corresponding to any load case or combination,
as well as envelopes. You can turn on and off the display of envelope functions
and set the position along the member where you want the results displayed.

Save diagrams
to the Drawings
Library

Associative diagrams can be saved to the Drawings Library. Drawings from
this library can be inserted into reports. After changing and recalculating the
model diagrams in the library and reports change accordingly.

The internal forces are related to the element local coordinate system, and the
positive sign conventions apply as in the figure above. The moment diagrams
are drawn on the tension side of the beam elements.

Displaying the internal forces of a frame:

Nx diagram Vz diagram

My diagram My min/max envelope

User’s Manual 229

If you click a beam element all six beam internal force components
are displayed in a diagram form.
You can display internal forces of more than one beam element if:
a) The local coordinate system of the elements are almost or entirely
identical. See... 2.15.14.3 Drawing/ Contour line angle
b) The local x orientation is the same.
c) The elements have the same material.

On selecting envelope or critical load combination, the selected beam internal
force minimum and maximum values of the intermediate cross sections will be
displayed.

You can display the diagrams corresponding to any load case or combination,
as well as envelopes. You can turn on and off the display of envelope functions
and set the position along the member where you want the results displayed.

Save diagrams
to the Drawings
Library

Associative diagrams can be saved to the Drawings Library. Drawings from
this library can be inserted into reports. After changing and recalculating the
model diagrams in the library and reports change accordingly.

Result Tables If the min/max values occur in a single location the concomitant values of the
afferent internal force components are displayed, or the symbol * (if there are
multiple locations). An occurrence of such a location is displayed.

See... 6.1.4 Result Tables

230 AxisVM 8+Release 4

6.1.7. Rib Element Internal Forces
Three orthogonal internal forces, one axial and
two shear forces (N
x
, V
y
, V
z
) and three internal
moments, one torsional and two flexural
(T
x
, M
y
, M
z
) are calculated at the nodes of each
element. The rib can be used independently
(not connected to a surface element),
or connected to a surface element.

The internal forces are related to the element local coordinate system
positioned in the center of gravity of the cross-section, and the positive sign
conventions apply as in the figure below. The moment diagrams are drawn
on the tension side of the beam elements.
If the rib is connected eccentrically to a shell element, axial forces will appear
in the rib and in the shell.

Displaying the internal forces of a ribbed plate:

Tx diagram My min/max envelope

Result Tables See... 6.1.4 Result Tables

6.1.8. Surface Elements Internal Forces
Internal forces The internal forces and the positive sign conventions of each surface element
type are summarized in the table below.

Surface elements
Membrane

nx
ny
nxy
Plate

mx
my
mxy
vxz
vyz

Shell

nx
ny
nxy
mx
my
mxy
vxz
vyz

User’s Manual 231

Displaying the internal forces of a ribbed plate:

Diagram Section line

Isoline Isosurface 2D

F
The x and y index of the plate moments indicates the direction of the normal
stresses that occur due to the corresponding moment, and not the rotation axis.
So, the mx moment rotates about the y local axis, while the my about the
x local axis.
The moment diagrams of plate and shell elements are drawn on the tension
side. On the top surface (determined by the local z direction) the sign is always
positive, on the bottom surface it is always negative.

Intensity variation The finite element method is an approximate method. Under normal
circumstances the results converge to the exact values as the mesh is refined.
The refinement of the mesh (the number of the elements used in the mesh),
the geometry of the elements, the loading and the support conditions,
and many other parameters influence the results. Therefore some results will
be relatively accurate whereas other results require the user to determine
if they meet the conditions of accuracy that he expects.

The intensity variation values are intended to give you help in identifying the
regions in your model (mesh) where it is possible that the accuracy of the
results is not satisfactory, without performing an additional analysis.
This method does not show that the results are good, but will highlight
intensity variations with high magnitudes, where you may want to check
and/or refine your mesh.
The allowable values of the intensity variation can be determined based on
practice.

F
In the case of plane strain membrane elements, n
z
≠ 0 and is not determined.
$
The internal forces can be displayed in diagram, section line, isoline
or isosurface forms.
The principal directions (α
n
, α
m
) can be displayed only in diagram form.
The direction vector color and size are determined based on the value of the
respective principal internal forces.
If the principal internal force is negative the corresponding direction vector
is bounded by two segments perpendicular to it.

Displaying the internal forces of supports in a frame and a shell structure:

Ryy moments ReR resultant forces

Ry edge forces ReR edge resultant forces

Result Tables See...6.1.4 Result Tables

6.1.10. Internal forces of line to line link elements and edge hinges
Internal forces AxisVM determines the nx, ny, nz forces and mx, my, mz moments for line to
line link elements and edge hinges. If any stifness component is set to zero the
related result component is zero and not displayed neither in the component
combo nor in result tables.

234 AxisVM 8+Release 4

6.1.11. Truss/Beam/Rib Element Stresses
The display modes for stress results are the same as for the internal forces.
The table of the stress results are similar to those of internal forces.

Beams / Ribs The following stress values are calculated in each stress point of each cross-
section of the beam/rib element:
Normal stress from tension/compression and bending is calculated disregard-
ing warping stress:
i
yz z y
yz y y z
i
yz z y
yz z z y
x
x
i x
y
I I I
I M I M
z
I I I
I M I M
A
N
S
2 2
,
−
+
−
−
+
+ ·
where y
i
, z
i
are the stress point coordinates. Positive stress value means ten-
sion in the cross-section.
Resultant shear stress is calculated from shear and twisting (Saint-Venant)
disregarding warping shear stress.

Φ
y
and Φ
z
are the shear stress functions for shear in y and z direction, ω is the
warping function.
For thin-walled cross-sections:
i
x
x
i
i x
x
i
z
x
z
i
y
x
y
i
t
I
M
m
s I
M
s A
V
s A
V
V +

,
`

.
|
+
,
`

.
|
∂
ω ∂
+
,
`

.
|
∂
Φ ∂
+

,
`

.
|
∂
Φ ∂
· ,
where the last two terms are the shear stress from twisting derived from shear
flow in closed and open subsections. m
i
is the distance of the centre of gravity
from the segment, t
i
is the wall thickness of the segment. ω, Φ
y
and Φ
z
are cen-
terline values.
Von Mises stress is defined as
2 2
, ,
3
i i x i o
V S S + ·
If a cross-section contains two or more separate parts V
i
és S
o,i
is not calculated.
Mean shear stresses:
y y mean y
A V V ·
,
,
z z mean z
A V V ·
,
,
if Ay, Az = 0 then Ay=Az=Ax.

Beam stresses Sminmax, Vminmax, Sominmax are minimum / maximum values
within the cross-section and displayed like internal forces.
You can click a beam/rib element to display stress diagrams. On the left the
minimum/maximum values along the line are displayed. Dragging the blue
line with the mouse the evaluation position can be changed. The axonometric
diagrams in the middle and the tables on the right show the stress distribution
within the section at the evaluation point.
Select more elements before clicking to display them in one diagram.
Continuous beams/ribs can be displayed in one diagram if conditions
described in section 6.1.5 are satisfied.

User’s Manual 235

You can display the diagrams corresponding to any load case or combination,
as well as envelopes. You can turn on and off the display of envelope functions
and set the position along the member where you want the results displayed.

Save diagrams
to the Drawings
Library

Associative diagrams can be saved to the Drawings Library. Drawings from
this library can be inserted into reports. After changing and recalculating the
model diagrams in the library and reports change accordingly.

F
Selecting envelope or critical combinations only one of the min and max
components will appear depending on the component. If extreme values are
located in one cross-section only you will see values of the other components as
well. Otherwise a ∗ will appear and the cross-section location will be the first
one.

Result Tables See... 6.1.4 Result Tables
6.1.12. Surface Element Stresses
The following stress components are calculated at each node of the element in
the top, center, and bottom fiber:

Component Membrane Plate Shell
s
xx

t
n
s
x
xx
·
x xx
m
t
s ⋅ t ·
2
6

x
x
xx
m
t t
n
s ⋅ t ·
2
6

s
yy

t
n
s
y
yy
· y yy
m
t
s ⋅ t ·
2
6

y
y
yy
m
t t
n
s ⋅ t ·
2
6

s
xy

t
n
s
xy
xy
· xy xy
m
t
s ⋅ t ·
2
6

xy
xy
xy
m
t t
n
s ⋅ t ·
2
6

s
xz

t
v
s
xz
xz
2
3
·
t
v
s
xz
xz
2
3
·
s
yz

t
v
s
yz
yz
2
3
·
t
v
s
yz
yz
2
3
·

F
In the case of plane strain membrane elements 0 ≠
zz
s , and is determined as:
) (
yy xx zz
s s s + ⋅ ·ν
In case of moments the x or y suffix refers to the direction of the section, therefore
mx moment will make the plate rotate around the local y direction and my
around the local x direction.

$
Stress values can be displayed as a diagram, section diagram, as isolines or
isosurfaces.
Result Tables See... 6.1.4 Result Tables

6.1.13. Influence Lines
Displays the internal force influence lines corresponding to the unit applied
forces PX, PY, PZ that act in the positive direction of the global coordinate axes.
An ordinate of the influence line represents the value of the respective internal
force that occurs in the respective cross-section caused by an applied unit force
at the position of the ordinate.

The resultant of all external loads with respect to the origin of the global
coordinate system is calculated (in the direction X, Y, Z, XX, YY, ZZ) for each
load case.
The unbalanced loads for each load case is also displayed (UNB) by its
components (in the direction X, Y, Z, XX, YY, ZZ). The unbalanced loads are
not appearing in the supports, therefore, if there are non-zero unbalanced load
components, it usually means that a part of the external loads are supported
by constrained degrees of freedom and not the supports.

F
It is recommended to check the unbalanced loads after each analysis run.

6.2. Vibration

Displays the results of a vibration analysis (mode shapes and frequencies).
You must specify the mode shape number.
The mode shapes are normalized with respect to the mass.

Displaying mode shapes:

Frame, first mode Frame, second mode

Plate, second mode Plate, sixth mode

238 AxisVM 8+Release 4

In the Info Window the following will appear:
f the frequency
ω the circular frequency
T the period
Ev the eigenvalue
Error: the relative Error of the eigenvalue

Iteration the number of iteration performed until convergence was
achieved
F
AxisVM stores the vibration analysis results corresponding to each case.

Result table See... 6.1.4 Result Tables
6.3. Buckling

Displays the results of a buckling analysis (buckling mode shapes and critical
load parameters).
In the Info Window the following will appear: Buckling of a frame:

Surface reinforcement can be calculated based on Eurocode 2. The calculation
of the reinforcement of membrane, plate, and shell elements is based on the
3
rd
stress condition. Reinforcement directions are the same as the local x and y
directions. The nominal moment and corresponding axial strengths
are determined based on the restricted direction optimal design.
F
The minimum reinforcement is not calculated. If the amount of reinforcement
that is calculated is less than the minimum reinforcement, the calculated values
are informative only, and are not based on the assumptions of an under
reinforced design.

User’s Manual 239

Result
components
mxD, myD,
nxD, nyD

design forces
axb: calculated reinforcement area at the bottom in x direction
ayb: calculated reinforcement area at the bottom in y direction
axt: calculated reinforcement area at the top in x direction
ayt: calculated reinforcement area at the top in y direction
xb: actual (applied) reinforcement at the bottom in x direction
yb: actual (applied) reinforcement at the bottom in y direction
xt: actual (applied) reinforcement at the top in x direction
yt: actual (applied) reinforcement at the top in y direction
wk(b) crack opening in the axis of bottom reinforcement
wk(t) crack opening in the axis of top reinforcement
wk2(b) crack opening at the bottom of the plate
wk2(t) crack opening at the top of the plate
wR(b) crack direction at the bottom of the plate
wR(t) crack direction at the top of the plate

Reinforcement
parameters

In the surface reinforcement design, the following parameters must be
assigned to the finite elements:

Materials Concrete material
Rebar material
Thickness h the total thickness used in the calculation

Unfavorable
eccentricity
It has to be added in case of Eurocode2.
Extra eccentricities will always be added to the actual value (calculated
from normal forces and moments) to increase the absolute value of the
excentricity.

F
The position of the reinforcement is defined as the distance between the edge of
the concrete and the axis of the rebar.

6.4.1.1. Calculation based on Eurocode 2
Plate If mx, my, mxy are the internal forces at a point, then the nominal moment
strengths are as follows:

- the moment optimum is:
! min
0
1
2
· ∆
· ∆
m
m

x y
m m ≥

Results AxisVM calculates the tension and/or compression reinforcements (for doubly
reinforced sections).
The following results are obtained at each point:

top
y
top
x
bottom
y
bottom
x
A A
A A
,
, ,

Error messages
F
The error message The section cannot be reinforced appears if:
c
top
s
bottom
s
A A A 04 . 0 > + ,
where A
c
is the concrete cross-section area.

Tables The following symbols are used in tables:
(-) compression reinforcement bar
??? the section cannot be reinforced in the corresponding direction
No special symbol is used for tension reinforcement.
User’s Manual 241

Membrane Only plane stress membranes can be reinforced.
If nx, ny, nxy are the internal forces at a point, then the nominal axial strengths
are as follows:

- the axial force optimum is:
! min
0
1
2
· ∆
· ∆
n
n

x y
n n ≥

Results AxisVM calculates the tension or compression reinforcements. Compression
reinforcement is calculated only in the points at which the axial compression
resistance of the section without reinforcement is lower than the compressive
design axial force.

The following results are obtained at each point:
axb, axt, ayb, ayt
Total reinforcement in x direction: Ax = axb + axt
Total reinforcement in y direction: Ay = ayb + ayt
F
The total amount of reinforcement necessary is Axa + Axf.

Error messages
F
The error message The section cannot be reinforced appears if:
c
top
s
bottom
s
A A A 04 , 0 > + ,
where A
c
is the concrete cross-section area.

Shell If nx, ny, nxy, mx, my, mxy are the internal forces in a point, than the design axial
forces and moments are established based on the reserve axial force optimum
and reserve moment optimum criterias that were emphasized, at the
membrane reinforcement and plate reinforcement description.
The program calculates the necessary tensile and compressive reinforcement.
Results The following values are provided as results:
axa, axf, aya, ayf
Total reinforcement in x direction: Ax = axa + axf
Total reinforcement in y direction: Ay = aya + ayf

Reinforcement of membranes, plates and shells are calculated according to the
three-layer method.
The internal forces (m
x
, m
y
, m
xy
, n
x
, n
y
, n
xy
) are calculated in the perpendicular
directions of the reinforcement.
The surface is divided into three layers. Membrane forces for the top and
bottom layers are calculated then design forces and the required amount
of reinforcement is determined.

Besides calculating the required reinforcement zones of concrete are checked
for shear and compression according to A, B and C cases.

Case A

Case B

Case C

Error message
The error message The section cannot be reinforced appears.
If the compressed zone of the concrete fails due shear forces.
If the compression principal stress is higher than f
cd
.
c
top
s
bottom
s
A A A 04 , 0 > + where A
c
is the concrete cross-section area.
Tables The following symbols are used in tables:
(-) compression reinforcement bar
??? the section cannot be reinforced in the corresponding direction
No symbol appears when tension reinforcement is required.

Medium layer
Bottom layer
Top layer
User’s Manual 243

6.4.2. Actual Reinforcement
Actual
Reinforcement

Lets you apply an actual reinforcement to the surface elements depending on
the calculated reinforcements.
Using the actual reinforcement you can perform a non-linear plate deflection
analysis.

The top and bottom reinforcements should be specified as follows:

Reinforcement

The actual reinforcement of the selected surfaces is shown in the tree on the
left. Selecting a reinforcement makes its parameters editable on the right.
Changing the values updates the tree.

Min. Thickness Min. Thickness displays the minimum thickness entered as surface
reinforcement parameter for the selected elements, and not the minimum
thickness of the elements.

F
The position of the rebar is defined as the distance between the side of the
concrete and the axis of the rebar.

Add and Delete The applied reinforcement is shown in a tree view on the left. By selecting a
reinforcement you can change its parameters in the right side. By selecting a
location (e.g. x Direction / Top Reinforcement) you can set a new
reinforcement on the right side and add it.

Use the Delete button (or [Del] key) to delete reinforcement or the Add button
(or [INS] key) to add reinforcement to a group. If you select a node of the tree
view the Delete button (or [Del] key) will delete all the reinforcements under
that node. The Add button (or [INS] key) will add reinforcement to the
corresponding group.

Max. Reinforcement
in Selection
In the Max. Reinforcement in Selection group box the maximum calculated
reinforcement values are displayed corresponding to different directions of the
selected elements.

After the assignment of the actual reinforcement
the program calculates the crack openings and
crack directions in the membrane, plate and
shell elements.

The direction of the reinforcement is relative to the surface element’s local
x and y axes.The program displays the crack openings in a color coded mode,
can draw the crack map and the crack angles.
The set of the parameters can be seen in the previous section.

Results In the table of results the following information can be found:

Aax, Aay actual reinforcement in x and y direction
wk crack opening at the axis of the rebar
wk2 crack opening at the edge of the slab
x
s2
position of the neutral axis relative to the edge on the compressed side
σ
s2
rebar stress
wR angle of cracking relative to the local x direction
nx, ny, nxy, mx, my, mxy surface forces and moments

F
A warning message will appear
if the calculated rebar stress is
higher than the characteristic
yield strength.
The calculation of crack opening
is based on the actual rein-
forcement assigned to the sur-
faces.

The program takes account of the fact that cracking is not perpendicular to any
of the reinforcement directions and calculates its angle relative to the x axis.

6.4.4. Non-linear deflection of RC plates

In case of the linear static analysis the plate deflection is calculated according
to the elastic theory. In fact the behaviour of RC plates is non-linear due to two
opposite effects. The actual reinforcement increases the bending strength but
cracking decreases it. The non-linear RC plate deflection analysis follows up
these two effects with the actual reinforcement.

The program performs a non-linear analysis in an iterative way using the
moment-curvature diagrams of RC cross-sections. The strength effect of the
tensile concrete is also taken into account.
This non-linear analysis is available based on Eurocode, DIN 1045-1 (German),
SIA-262 (Swiss), NEN (Dutch), MSz (Hungarian) and STAS (Romanian)
design codes.

The main steps of a plate deflection calculation are
1.) performing a linear analysis of the plate
2.) calculating the required reinforcement
3.) applying the actual reinforcement
4.) performing a non-linear analysis of the plate

246 AxisVM 8+Release 4

F
When you start the non-linear analysis, check the Use actual reinforcement in the
calculation checkbox.

AxisVM calculates the shear resistance of the reinforced plate or shell without
shear reinforcement, the normal shear force and the difference between them.

2 2
yz xz Sz
v v v + · is the resultant shear force, where v
xz
, and v
yz
are the shear
force components in planes with normals in the local x and y
direction.

) / arctan(
xz yz
v v · φ is the angle of the normal of the plane, in which resultant
shear force of q
Rz
acts.

2 / ) (
y x
d d d + · is the average effective height.

φ ρ φ ρ ρ
4 4
sin cos ⋅ + ⋅ ·
y x l
is the reinforcement ratio perpendicular to the
plane in which q
Rz
acts.
ρ
x
and ρ
y
are rebar ratios calculated from tension reinforcement in x and y
directions of the reinforcement.
F
The calculation of the shear resistance is based on the actual reinforecement
assigned to the surfaces.

$
The V
Rdc
shear resistance and the difference between actual shear force and
the shear resistance (v
Sz
–V
Rdc
) can also be displayed with isolines and
isosurfaces.

User’s Manual 247

6.4.6. Column Reinforcement

The reinforced column check can be performed based on the following
design codes:
Design Codes Eurocode 2: EN 1992-1-1:2004
DIN: DIN 1045-1:2001-07
SIA: SIA 262:2003

Commands for editing are the same as in the main window.
See... 2.5 Using the Cursor, the Keyboard, the Mouse.

On Reinforcement bars tab the cross-section can be choosen, material
parameters of the concrete column and the rebars, buckling lengths of the
column can be set and rebars can be placed.
After clicking the Column Check tab N-M strength interaction diagrams
are calculated.

Open

Opens a new cross-section or reinforcement.

F
Only cross-sections with graphics data can be opened.
Save

Saves the reinforcement under a name for further use.

Save diagram to the Drawings Library.

248 AxisVM 8+Release 4

Define
Reinforcement
The following icons are available on the Define Reinforcement menu:
Parameters

Lets you specify the parameters for calculation of the load-moment strength
interaction diagram.
The unfavorable eccentricity increments determined based on the buckling
parameters are displayed in the internal force check table.

Reinforcement Bars
To a point Covering

Generates a reinforcement bar with a specified diameter to the location of the
cursor.
If the cursor is on a corner or on the contour line the reinforcement will be
generated taking into account the concrete cover.

By spacing

Inserts evenly N+1 new rebars between two selected points.

On circular arch

Inserts evenly N+1 new rebars between a selected starting point and an end-
point of a circular arch.

Diameter

Lets you define or modify the diameter of a rebar.
To modify, select the rebars and than the enter the diameter or select a value
from the list.

Covering

Lets you define or modify the concrete covering.
In this case the concrete cover is the distance from the
extreme fiber to the rebar!
Modifying the geometry of the rebars:

1. Move the cursor over the centroid of the rebar.
2. Use the left 8 button (keep depressed) to move the
rebar to its new location, or, enter its new coordinates
numerically in the coordinate window.

N

The division number which defines the number of rebars as N+1.

Translate

Creates new rebars by copying existing ones by translation.

Rotate

Creates new rebars by copying existing ones by rotation.

Mirror

Creates new rebars by mirroring existing ones.

User’s Manual 249

Modifying the geometry of the rebars:

1. Move the cursor over the centroid of the rebar.
2. Use the left 8 button (keep depressed) to move the rebar to its new
location, or, enter its new coordinates numerically in the coordinate
window.

Column Check Calculates the interaction diagram based on the cross-section properties and
reinforcement parameters and determines the eccentricity increments for the
forces in the selected columns (or any N
x
,

M
ya
,

M
za
, M
yf
,

M
z f
values) based on
the given buckling parameters and according to the requirements of the
current design code.
Calculates N
xd
,

M
yd
,

M
zd
design forces using the eccentricity increments and
checks if these points are within the interaction diagram.
The display of the diagram can be set in the Display Parameters window.

Select display mode by clicking a radio button in the Display Mode group box.
It has the same effect as selecting it from the dropdown list.
Select axial force values to use when drawing the 3D interaction diagram
(N-M Surface) from the check list.
In the Labels group you can turn on and off axial force labeling, the display of
graphic symbols for internal forces of selected columns in the N-My-Mz space
and display options for the cross-section display mode.

This display mode can be used with cross-sections that are symmetric.
You can display the design values of the internal forces, by enabling the
Write Values to check-box.
The design values of the internal forces are displayed as follows:

Internal forces The Column Internal Force Check table contains the maximum normal forces
and moments at the top and bottom end of the selected columns and different
eccentricity values.

On N-M
R
strength interaction diagrams and on
load eccentricity limit curves points represent
these design loads.
Custom force and moment values can also be
entered into the table. These points will be
displayed in the N-M
R
strength interaction
diagrams and in the load eccentricity limit
curves.
Signs of the foces and moments are deter-
mined according to the picture.

Rebars thinner than 1/12 of the stirrup distance will be ignored for
compression.

User’s Manual 253

6.4.6.1. Check of reinforced columns based on Eurocode 2
The design moments in bending directions are
d d d
e N M ⋅ ·
where N
d
is the normal force in the column and
2
e e e e
i e d
+ + · is the
standard eccentricity in the given bending direction.
e
0
= M
I
/N
d
initial eccentricity calculated from the first order force and
moment.
If moments at the top and bottom end of the column are different,
a substitute initial eccentricity will be determined:
¹
'
¹
¹
'
¹ +
·
a
b a
e
e
e e
e
4 . 0
4 . 0 6 . 0
max and
b a
e e ≥ ,
where e
a
and e
b
are the initial eccentricities at the ends of the column.

AxisVM checks whether the calculated design loads (M
dy
, M
dz
, N
d
) are inside
the N-M strength interaction diagram. If it is not satisfied in any of the design
situations, the column with the given cross-section and reinforcement fails.

e
0ay
, e
0az
, and e
0by
, e
0bz
are the initial eccentricities at the bottom and top end of
the column.

The calculation takes the following assumptions:
σ,ε diagrams:

254 AxisVM 8+Release 4

6.4.6.2. Check of reinforced columns based on DIN1045-1
Design moments in bending directions are
d d d
e N M ⋅ ·
where N
d
is the normal force in the column and
2 0
e e e e
a d
+ + · is the critical
eccentricity in the given bending direction.
e
0
= M
dI
/N
d
initial eccentricity calculated from the first order force and
moment.
If moments at the top and bottom end of the column are different,
a substitute initial eccentricity will be determined:
¹
'
¹
¹
'
¹ +
·
a
b a
e
e
e e
e
4 . 0
4 . 0 6 . 0
max and
b a
e e ≥ ,
where e
a
and e
b
are the initial eccentricities at the ends of the column.

AxisVM checks whether the calculated design loads (M
dy
, M
dz
, N
d
) are inside
the N-M strength interaction diagram. If it is not satisfied in any of the design
situations, the column with the given cross-section and reinforcement fails.

e
0ay
, e
0az
, and e
0by
, e
0bz
are the initial eccentricities at the bottom and top end of
the column.

e
1d
= M
dI
/N
d
initial eccentricity calculated from the first order force and
moment.
If moments at the top and bottom end of the column are different, a
substitute initial eccentricity will be determined:
¹
'
¹
¹
'
¹ +
·
a
b a
e
e
e e
e
4 . 0
4 . 0 6 . 0
max and
b a
e e ≥ ,
where e
a
and e
b
are the initial eccentricities at the ends of the column.

AxisVM checks whether the calculated design loads (M
dy
, M
dz
, N
d
) are inside
the N-M strength interaction diagram. If it is not satisfied in any of the design
situations, the column with the given cross-section and reinforcement fails.

e
ay
, e
az
, and e
by
, e
bz
are the initial eccentricities at the bottom and top end of
the column.

F
The beams are structural elements, with one dimension (the length) significantly
greater than the dimensions of the cross section, loaded in bending and shear, and
axial force is zero or of a small, negligible value.
The beam reinforcement design module can be applied to beam structural
elements modeled by beam or rib finite elements, that have the same material
and constant or variable rectangular or T cross sections, assuming that the load
is applied in the symmetry plane of the cross section.
The computed longitudinal top and bottom reinforcement are of the same steel
grade, while the stirrups could have steel grade different from the longitudinal
ones.

Variable
cross-section

The change in shear force due to vari-
able cross-section is taken into ac-
count. Where sign of the moment
does not change a simple rule can be
applied: if section height changes the
same way as the moment along the
line shear capacity increases other-
wise it decreases.

Shear force is modified by α · ∆ sin 2
yd s
f A V , where
s
A is the longitudinal
tension reinforcement area, α is the angle between the extreme fiber and the
centerline. Longitudinal reinforcement is assumed to be parallel with the
extreme fiber.

2. Determination of spacing of vertical stirrups considering shear forces about
y or z axis (Vy or Vz) and the twisting moment (Tx).

The axial force is not taken into account. If the axial force cannot be neglected,
the use of the Column Design module is recommended.
Bending and shear/twisting is analyzed separately, however the longitudinal
tensile reinforcement is taken into account in the determination of the shear
capacity.
The increase in the tension in the longitudinal rebars due to the shear cracks
are accounted by shifting the moment.
F
AxisVM performs only design procedures listed in this section.
Any other requirement shall be fulfilled by the user, following the requirements of
the design codes, and corresponding other regulations.
The Beam Design module does not check the effect of biaxial bending, lateral
torsional buckling transversal stresses due to direct application of point loads, or
any interaction involving these.
The module cannot be applied to the design of short cantilevers.
User’s Manual 257

Define of size of
support

Clicking on the support the following dialog window is displayed:

Lets you specify the segments each side of the
support that will be not included in the
calculations. The internal forces are linearly
interpolated within the segments.
.
The diagram below shows the moment/shear force reduction above supports:

258 AxisVM 8+Release 4

Beam parameters

Design Internal
Forces
Selection of the z-x or y-x plane of the internal forces used for design.

Stirrup
Stirrup legs: lets you set the number of stirrup legs subject to shear.
F
Concrete coverings (ub, ut): distance between the centroid of rebar and the
corresponding extreme fiber of the concrete.

u
b
: the distance of the center of the
bottom rebar from the edge of the
cross section.
u
t
: the distance of the center of the
top rebar from the edge of the
cross section.

Longitudinal rein-
forcement from
bending
$
On the longitudinal reinforcement diagram the tension reinforcement
is displayed in blue, the compression reinforcement in red, and the minimal
reinforcement according to the design code in gray.

Longitudinal rein-
forcement from tor-
sion
$
The longitudinal reinforcement diagram is displayed in purple.
The longitudinal reinforcement from torsion should be placed uniformly
around the cross-section contour.

260 AxisVM 8+Release 4

Stirrup spacing
$
The allowable maximum stirrup spacing is displayed in black, the calculated
spacing in blue, and the minimal spacing according to the design code in gray.

The design is based on the following values of design shear resistance:

V
Rd,c

Design shear resistance of the cross-section without shear
reinforcement.
V
Rd,max
Maximum shear force that can be transmitted without the failure of
the inclined compression bars.
V
Rd,s
Design shear resistance of the cross-section with shear
reinforcement.

T
Rd,c

Design torsional resistance of the cross-section without shear
reinforcement.
T
Rd,max
Maximum torsional moment that can be transmitted without the
failure of the inclined compression bars.
AxisVM calculates the shear & torsion reinforcement assuming that shear crack
inclination angle is 45°. The relation between the capacity of inclined
compression concrete bars and the design values is checked.

By changing the shear crack inclination angle the compressed concrete beams
gets more load while shear reinforcement gets less. The actual saving depends
on the design rules.
If the user chooses the variable angle truss method, AxisVM determines the
direction of the shear crack between 21,8° (ctgˆ=2,5) and 45° (ctgˆ=1) before
the calculation of the reinforcement so that the exploitation of the inclined
concrete compression beams reach its maximum (at most 100%). The shear
crack inclination angle is increased in small steps to meet the requirement
1
max , max ,
≤ +
Rd
Ed
Rd
Ed
T
T
V
V

AxisVM calculates
longitudinal
reinforcement according
to this figure:

Limit stress is assumed in the rebars. The depth of the compressed zone will be
less than
cu s
c cu
d x
ε ε
ε ε
−
−
⋅ ·
1
1
0
.
If calculation results in a greater depth than x
0
, a compression reinforcement is
applied, but the sum of the area of reinforcement on the compression and on
the tension side cannot exceed 4% of the concrete cross-section area.

The required top and bottom reinforcement along the beam and the moment
diagram shift is calculated for each load case.

262 AxisVM 8+Release 4

Due to inclined cracks tension reinforcement is designed for a force greater
than calculated from M/z.
This is taken into account by different design codes by shifting the moment
diagram.

Minimum (M
min
≤ 0) and maximum (M
max
≥ 0) values of the moment diagram
and the corresponding reinforcement on tension and compression side is
determined. Tension reinforcement is displayed in blue, compression
reinforcement in red, the minimal tension reinforcement required by the
design code appears in grey.

Compression reinforcement has to be considered even if tension reinforcement
is the critical one, as longitudinal rebars thinner than 1/12 of the stirrup
distance has to be ignored when determining the compression rebar diameter
or the stirrup spacing.

The design is based on the following three values of design shear resistance:

V
Rd,ct

Design shear resistance of the cross-section without shear
reinforcement.
V
Rd,max
Maximum shear force that can be transmitted without the failure of
the inclined compression bars.
V
Rd,sy
Design shear resistance of the cross-section with shear
reinforcement.

The software calculates for each load case and cross section the lower and
upper reinforcement, and the value of the moment shifting.
264 AxisVM 8+Release 4

Due to oblique cracks the tension reinforcement is designed for a tension force
greater than calculated from M / z.
This is taken into account by design codes by shifting the moment diagram
(DIN 1045-1 13.2.2)
Minimum (M
min
≤ 0) and maximum (M
max
≥ 0) values of the moment diagram,
and the corresponding tension and compression reinforcements
are determined. On the reinforcement diagram the tension reinforcement
is displayed in blue, the compressive in red, and the minimal tension
reinforcement according to the design code in grey.
The compression reinforcement is necessary even if the tension reinforcement
is the critical, because at the determination of the compression reinforcement
diameters and stirrup spacing is taken into account that only the 1/12 of the
stirrup spacing or longitudinal rebars with greater diameter are included.

F
The software is sending warning message and does not draw any reinforcement
diagram in the following cases:
Message
The cross section is not acceptable for shear/torsion
Event Any of the following conditions is not satisfied:
Ed max Rd,
V V ≥ or 1
2
max
2
max
≤
]
]
]
]

+
]
]
]
]

Rd,
Ed
Rd,
Ed
V
V
T
T

Solution Increase the cross section of the concrete, or/and the concrete grade.

Message
The cross section is not acceptable for bending (As + As2 > 0.08 * Ac)
Event The cross sectional area of the longitudinal reinforcement is greater than 8% of the
concrete cross section
Solution Increase the cross section of the concrete, or/and the concrete grade, or/and the
steel grade.

The shear reinforcement design is based on three values of the shear
resistance:

V
Rd
The shear resistance of the cross section without shear
reinforcement.
V
Rd,c
The maximum shear force that can be transmitted without the
failure of the assumed compression bars.
V
Rd,s
The shear resistance of the cross section with the shear
reinforcement.

The limit stress is developing in the reinforcement. The depth of the
compressive concrete zone will exceed
u c s
c u c
d x
2 1
2 2
0
ε ε
ε ε
−
−
⋅ · , where ε
s1
= f
yd
/ E
s
.
If from the calculation a greater height than x0 is obtained, compressive steel
cross section is applied, but the sum of the compressive and tensile steel cross
section cannot exceed 8% of the concrete cross section.
The software calculates for each load case and cross section the lower and
upper reinforcement, and the value of the moment shifting.
Due to oblique cracks the tension reinforcement is designed for a tension force
greater than calculated from M / z.
This is taken into account by shifting the moment diagram.
Minimum (M
min
≤ 0) and maximum (M
max
≥ 0) values of the moment diagram,
and the corresponding tension and compression reinforcements
are determined. On the reinforcement diagram the tension reinforcement
is displayed in blue, the compressive in red, and the minimal tension
reinforcement according to the design code in grey.
The compression reinforcement is necessary even if the tension reinforcement
is the critical, because at the determination of the compression reinforcement
diameters and stirrup spacing is taken into account that only the 1/12 of the
stirrup spacing or longitudinal rebars with greater diameter are included.

F
AxisVM sends a warning message and does not draw any reinforcement diagram
in the following cases:

Message
The cross section is not acceptable for shear/torsion
Event If the efficiency of concrete cross-section greater than 1.
Solution Increase the cross section of the concrete, or/and the concrete grade.

User’s Manual 267

6.4.8. Punching Analysis

Punching shear control perimeters are determined based on the column cross-
section and the effective plate thickness. Plate edges and holes are taken into
account if they are closer to the column than six times the effective plate
thickness. If column cross-section is concave a convex section is used instead.

Punching analysis can be performed based on the following design codes:

Design Codes Eurocode 2: EN 1992-1-1:2004
DIN: DIN 1045-1:2001-07

After clicking the tool button select a column or a support with stiffnesses cal-
culated from column parameters for analysis (if a rib element is connected to
the column within the plane of the plate, analysis cannot be performed).
The following parameters can be set:

Materials

Concrete,
Rebar steel
Concrete and reinforcing steel grade used in calculation. These parameters
are taken from the actual model by default and can be changed here.

Total plate
thickness (h)
Plate thickness is taken from the actual model by default and can be changed
here, if By reinforcement parameter is turned off. In the info window the
minimum mushroom head thickness is displayed as H1. The minimum mush-
room head without punching shear reinforcement is displayed as H2.

Parameters

Shear reinforcement
angle
Angle between the plate and and the punching shear rebars (45°-90°).

*For structures where the lateral stability does not depend on frame action
between the slabs and the columns, and where the adjacent spans do not
differ in length by more than 25%.

Take soil reaction
into account
If this option is checked soil reaction within the rebar circle is considered when
calculating the punching force. This effect increases with the radius and
can reduce the size of the necessary reinforcement area. Its values per rebar
circles are listed in the Punching Analysis Results dialog.

Loading... Loads the saved parameters of punching

After entering all parameters control perimeters will appear and the required
number of punching rebars is displayed in the info window.

$
AxisVM calculates the effective parts of the control perimeter based on plate
edges and holes. Continuous lines show that reinforcement is needed.
AxisVM displays the required amount of reinforcement for each line. The info
window shows the amount of critical punching reinforcement.
When calculating the length of the critical perimeter it is assumed that rebar
spacing on the perimeter is not above 2d but the fulfillment of this requirement
is not checked. If this requirement is not met, the user should choose a smaller
diameter or place additional rebars.

Results for the critical perimeter are calculated first (these are displayed in the
Punching analysis results dialog). Then the required amount of reinforcement is
determined for reinforcement circles defined in the parameters dialog.
The critical perimeter is red, reinforcement circles are black. Dashed line shows
the perimeter where the distance of points from the column is six times the
effective plate thickness.

A thin blue line shows the perimeter where no punching reinforcement is
needed. This is also the outline of the mushroom head which can be designed
with thickness H2 and without punching reinforcement.
A thick blue line shows the perimeter where the critical punching force
exceeds the compressing strength of the concrete so the plate with the original
thickness cannot be properly reinforced. This is the outline of the mushroom
head which can be designed with thickness H1 and with punching reinforce-
ment. Punching capacity can be increased by setting the plate thicker, using a
better concrete grade or columns with bigger cross-section area.

Saves the drawing into the Drawing Library.

Loads a saved punching parameter set.

Saves the current punching parameters under a name. You can load back the
saved parameters with the button Loading... on Punching Parameters Dialog.

Punching parameters dialog.

Inflates the plate boundary so that the entire column cross section is within the
boundary.

Fits the diagram to the window.

User’s Manual 269

Column local coordinates are used.

Global coordinates are used.

Turns on and off the display of rebar circles.

6.4.8.1. Punching analysis based on Eurocode2
The required punching reinforcement is calculated based on the following
principles:
The column-plate connection does not fail if the specific shear force is less than
or equal to the design value of the maximum punching shear resistance along
the control section and the design value of the punching shear resistance of
the plate with punching shear reinforcement:
max , Rd Ed
v v ≤ and
cs Rd Ed
v v
,
≤
v
Ed
design value of the specific shear force
v
Rd,max
the design value of the maximum punching shear resistance along the
control section
v
Rd,cs
the design value of the punching shear resistance of the plate with
punching shear reinforcement
d u
V
v
i
Ed
Ed
⋅
⋅ · β ,
where u
i
is the length of the control perimeter, d is the mean effective thickness
of the plate.
270 AxisVM 8+Release 4

6.4.8.2. Punching analysis based on DIN 1045-1
The required punching reinforcement is calculated according to the following
principles:
The column-plate connection does not fail if the specific shear force is less than
or equal to the design value of the maximum punching shear resistance along
the control section and the design value of the punching shear resistance of
the plate with punching shear reinforcement:
Rd sd
v v ≤
The design value of the specific shear force is
d u
V
v
sd
sd
⋅
⋅ · β , where β is a factor
expressing additional stress due to eccentric forces.
DIN 1045-1 assumes that the critical section is at a distance of 1,5d from the
edge of the cross-section.

r
1
: distance between the first rebar circle and
the convex column edge
A
sw
: punching reinforcement area on the critical
control perimeter
N
sr
: number of reinforcement circles

Warnings and error messages

Message Compression force in plate is too high.
Event The applied force is so high that the concrete plate fails irrespectively of the
reinforcement.
Solution The most efficient solution is to increase plate thickness.
The critical punching area can be extended by increasing plate thickness and/or
column size (reducing the design value of the specific shear force this way).
Choose a higher grade concrete.

6.5. Steel design

6.5.1. Steel beam design
EUROCODE 3 The steel beam design module can be applied to the following shapes:

Other type of shapes can not be designed with the module.
The class of the cross-sections should be of Class 1, Class 2, or Class 3.
Cross-sections belonging to Class 4 can not be designed with the module.
It is assumed that the cross-sections are not containing holes, and are made of
plates with a thickness less than or equal to 40 mm.
The cross-section is considered constant along the structural member, double
symmetric, and loaded in the shear center.

F
The program performs only the checks listed below. Any other check required by
the code (torsion, connection design, transversal actions, etc.) shall be performed
by the designer based on the design code.
It is assumed that the local z axis of the cross-sections with a web is parallel
with the plane of the web.

User’s Manual 273

Classes of Cross-
Sections
The program is identifying the class of the cross-section (EC3 5.3.2) based on
Table 5.3.1, considering uniform compression or bending only.

Axial Force-
Bending-Shear
The member can be in tension or in compression. If the shear force greater
than 50% of the shear resistance EC3 5.4.9, 5.4.7 is applied, or if less than 50%
the EC3 5.4.8 is used in the calculation.
For Class 1 and Class 2 cross-sections:

1
, ,
,
, ,
,
,
≤ + +
Rd z pl
Sd z
Rd y pl
Sd y
Rd pl
Sd
M
M
M
M
N
N

For Class 3 cross-sections:

1
, ,
,
, ,
,
≤ + +
fyd z el
Sd z
fyd y el
Sd y
fyd
Sd
W
M
W
M
A
N

Compression-
Bending-Buckling
The check is performed based on EC3 5.5.4 (5.51 and 5.53).
For Class 1 and Class 2 cross-sections:

Axial Force-
Bending-Lateral
Torsional Buckling
It is assumed that the cross-section is constant, double symmetric, and loaded
in the shear center. When determining the lateral-torsional buckling resistance
the value of k (EC3 F1.2) is taken equal with the lowest of K
z
(buckling length
factor) and 1. The weak axis should be the z local axis.
The check is performed based on EC3 5.5.4 (5.52 and 5.54).

For tensile axial force, the check is performed using the effective moments
based on EC3 5.5.3.

Shear /y The check is performed based on EC3 5.4.6, EC3 5.6.7.2 (5.20 and 5.66b).

1
, ,
,
≤
Rd y pl
Sd y
V
V

Shear /z The check is performed based on EC3 5.4.6, EC3 5.6.7.2 (5.20 and 5.66b).

1
) , ( min
, , ,
,
≤
Rd ba Rd z pl
Sd z
V V
V

Web Shear-
Bending-Axial Force
The check is performed for cross-sections with web based on EC3 5.6.7
assuming that the web is parallel with the local z axis.

1
,
,
≤
Rd f
Sd g
M
M

The simple post-critic method is applied.

Design
Parameters
For the design based on Eurocode 3, the following design parameters should
be defined and assigned to the structural members:

α
cr
Is the (smallest) critical elastic buckling load multiplier corresponding to a load
case or combination that includes all the vertical loading.
If α
cr
<4 a second order analysis is the only allowed for the determination of
displacements and internal forces.

User’s Manual 275

Stability
Parameters

Buckling (flexural) Ky, Kz: buckling length factor corresponding to the z and y axis, based on
EC3 5.2.6 and EC3 5.5.1.5.
If a support is continuous along the member, constraining the buckling about
an axis, the corresponding buckling length factor could be taken as nearly zero.
In a similar case, when there are intermediate supports, constraining the
buckling about an axis, the buckling length factor could be taken as the ratio of
the corresponding buckling length (between the intermediate supports)
and the length of the structural member.

Lateral Torsional
Buckling
Κ
ω
: is a factor related to the constrain against warping. Its value must be
between 0.5 and 1.
- if warping is not constrained it is 1.0.
- if warping is constrained at both ends of the beam, it is 0.5.
- if warping is constrained at one of the ends of the beam, it is 0.7.
See in detail: Appendix F1 of EC3 1993-1-1:1995.

C
1
, C
2
: are factors depending on the ratio of the end moments of the structural
element, on K
z
factor, and on the type of loading. The user can enter a value
for C
1
, or request an automatic determination. In the automatic mode, the
value of C
1
is taken 1 if K
z
is not equal with 1, or an intermediate moment is
larger than the larger end-moment, or if there are any transversal loads
applied. The automatic mode will take a value for C
1
based on EC3 F1.2 using
the formula F3, and assumes that the no external load is applied (Z
a
= 0) based
on EC3 F1.2, and will not ask for a value for C
2
.
In the case of a cantilever, C
1
shall be taken as 1, and the Auto mode can not be
used (the program can not determine if a structural member is a
cantilever).When external loads are applied to the structural member, a value
for C
2
shall be entered when Z
a
is not equal to 0, based on EC3 table F1.2.
Z
a
: is the z coordinate of the point of application of the transversal load
(relative to the center of gravity of the cross-section), based on EC3 Figure F1.1.

Web Shear
Buckling
For shapes with webs, the web can be supported or not with stiffeners:

No Stiffeners: assumes no transversal stiffeners along the struc-
tural member.
Transversal Stiffeners: there are transversal stiffeners at distance a each
from the other along the structural member.
In any cases the program assumes that there are transversal stiffeners at the
ends of the structural members (e.g. at the supports).

Steel structural
elements
The design is performed on structural elements that can consist of one or more
finite elements (beams and/or ribs). A group of finite elements can become a
structural element only if the finite elements in the group satisfy some
requirements checked by the program: to be located on the same straight line,
to have the same material, cross-section, and to have parallel local coordinate
systems.
The program allows two methods to define structural members as follows:
F
Structural elements for steel design are not the same as the structural members
See... 3.2.10 Find structural members

Any node of a selection set of finite elements, where an other finite element
is connected will become an end-point of a steel structural element within the
selection set of finite elements.

276 AxisVM 8+Release 4

Diagrams You can display the diagrams corresponding to all the checks by clicking on
the structural member.

F Assumptions:
- The beam and column cross-sections are rolled or welded I shapes.
- The beam end plate connect to the flange of the column.
- The pitch range of the beam is beetwen ± 30°.
- The cross-section class should be 1, 2 or 3.
- The normal force in the beam should be less than 0.05* N
pl,Rd
The program checks if these requirements are met.

User’s Manual 277

The steps of the
design
Select the beam and one of its end nodes.
(We can select several beams in one process if the selected beams have the
same material and cross-section properties and connected columns also have
the same material and cross-section properties.)

Click on the Joint Design icon.
The Bolted Joint Designer will appear:

Lets you assign the parameters of the joint in three steps.
Bracings We can assign horizontal, diagonal bracing plates and web thickening plates to
increase the strength of the connection.
Horizontal bracings

Web shear area The program calculate the web shear area including the thickening plate area.
If there is a hole in the web near to the connection you can decrease this value
in the data field depending on the hole size.

278 AxisVM 8+Release 4

End plate

Parameters of the end plate:
- thickness
- material
- welding thickness
- width of the end plate (a)
- height of the end plate (c)
- distance between top flange of
the beam and top of the end
plate (b)
- bolts in the extension of the end
plate

Bolt rows can be assigned to the tensile part of the end plate.

Bolts

The program places bolts in two columns symmetrical to the beam web.
The same type of bolts is used in the connection.
Bolt parameters:
- size
- material
- number of rows
- distance of bolt columns (d)

User’s Manual 279

In case of automatic positioning of bolts the program places bolt rows in equal
distances. The program checks the required minimal distances between bolts
and from the edge of plates.
Turn off the option Use default positions to place the bolt rows individually.
F
An error message will appear if the distances does not meet the requirements.

Minimal bolt distances are checked based on EC2:

1. Between bolts: 2,2 d
2. From edge of plate 1,2 d
3. In a direction perpendicular to the force 1,2 d

Results When we click on the Result tab AxisVM calculates the Moment-curvature
diagram, the design resistant moment (M
rD
) and the initial strength of the
connection (S
j,init
).

F
A warning message will appear if the resistant moment is less than the design
moment. The calculation method considers shear forces and normal forces
together with the moments. As a consequence we can get different resistant
moments (M
rD
) for the same connection depending on the load cases
(or combinations). Therefore AxisVM checks the M
rD
• M
sD

condition in all
load cases.

IconBar

Load the connection parameters.

Save the connection parameters. Saved parameters can be loaded and assigned
to other beam-end joints later.

First, select the surface elements, and then select the supported edges, to
define line support elements.
If you choose relative to edge support conditions, then the edge will represent
the x direction, and the y direction will be perpendicular to the edge in the
surface plane (according to the right-hand rule), and the z direction will be
perpendicular to the surface plane.

3.) Define the nodal degrees of freedom.

ð
Nodal DOF

Select all nodes to define degrees of freedom. Choose the
‘Plate in X-Y plane’ from the list.

286 AxisVM 8+Release 4

Loads
1.) Define load cases and combinations.

ð
Load case
and
load group

ð
Combination

2.) Apply loads (nodal, line, surface, dead load).

ð
Nodal

ð
Plate

ð
Plate

ð
Plate

ð
Plate

3.) Select domain, which have the same load.
The direction of distributed load is perpendicular to the plane of the surface,
and the sign of the load is the same as of the local z axis of the plate
(for example: p
z
=-10.00 kN/m
2
).

First, select the surface elements, and then select the supported edges,
to define line support elements.
If you choose relative to edge support conditions, then the edge will represent
the x direction, and the y direction will be perpendicular to the edge in the
surface plane (according to the right-hand rule), and the z direction will be
perpendicular to the surface plane.

6.) Define the nodal degrees of freedom.

ð
Nodal DOF

Select all nodes to define degrees of freedom. Choose the
‘Membrane in X-Z plane’ from the list.

Loads
1.) Define load cases and combinations.

ð
Load case
and
load group

ð
Combination

2.) Apply loads (nodal, line, surface, dead load).

ð
Nodal

ð
Membrane

ð
Membrane

ð
Membrane

ð
Membrane

User’s Manual 289

Select the elements, which have the same load.
The direction of distributed load is determined in the local x-y direction of the
membrane (for example: p
y
= -10.00 kN/m
2
).

2.) Apply all the gravitational loads that you want to account as masses in the
vibration analysis that precedes the static analysis.

Analysis/1

1.) Perform a vibration analysis. Vibration mode shapes for earthquake analysis
are usually requested as 3 for in-plane structures and 9 for spatial structures
are requested.

Include the gravitational load case described at Loads/1 point in the vibration
analysis, and set the Convert loads to mass check-box enabled.

290 AxisVM 8+Release 4

Loads/2
1.) Set a seismic load case.

ð
Load

2.) Specify the parameters of the seismic loads.

ð
Seismic

Analysis/2

1.) Start a linear static analysis.

2.) When generating the seismic type load cases, two are included. One “+” with
values included as positives, and one “-” with values included as negatives.
In addition the results corresponding to each vibration mode shape are
provided (corresponding to load cases with 01, 02, ….n suffixes), that can be
used in the generation of further combinations or of critical combinations.
See… 4.10.20 Seismic Loads

animation. Minimum Recommended Memory (RAM) Video adapter and monitor Hard disk Mouse or other pointing device Printer Operating system 64 Mbytes XGA 1024x768 with HI-Colors 100 Mbytes of free space Required Windows compatible laser or inkjet printer Windows 95/98/ Windows Millennium/Windows NT/ 2000/XP If available RAM exceeds 2 GB.
How to Use AxisVM
Welcome to AxisVM!
AxisVM is a finite-element program for the static. vibration. WMF. diagram. customizable tabular reports. Documentation is always part of the analysis. the limit of 2 GB per application can be increased to 3 GB by editing C:\boot. TXT. so you can experience maximum productivity with AxisVM. In addition data and graphics can be easily exported (DXF. you will receive graphical verification of your progress. EMF. AxisVM provides direct.User’s Manual
13
2. automatic meshing. DBF). JPG.
Analysis Postprocessing
Documentation
2. report. and perform further calculations using those results. import/export CAD geometry (DXF). Static. AxisVM can linearly combine or envelope the results. Preprocessing Modeling: geometry tools (point. element and load tools. AxisVM provides powerful visualization tools that let you quickly interpret your results. and buckling Displaying the results: deformed/undeformed shape display. Multi-level undo/redo command and on-line help is available. HTML. Enter the /3GB switch this way: [boot loader] timeout=30 default=multi(0)disk(0)rdisk(0)partition(1)\WINNT [operating systems] multi(0)disk(0)rdisk(0)partition(1)\WINNT="????" /3GB where ???? stands for the full name of the operating system. and a graphical user interface enhances the process and simplifies the effort.1.ini. lines. RTF. BMP. high quality printing of both text and graphics data to document your model and results. interface to architectural design software products like Graphisoft’s ArchiCAD via IFC to create model framework directly. After your analysis. Hardware Requirements
The table below shows the minimum/recommended hardware and software requirements. AxisVM combines powerful analysis capabilities with an easy to use graphical user interface. and numerical tools to search. and isoline/surface plots. It was developed by and especially for civil engineers. depending on the model size
. 1 GB or more XGA 1280x1024 with HI-Colors or more 2 GB of free space. material and cross-section libraries. The results can be used to display the deformed or animated shape of your geometry or the isoline/surface plots. and buckling analysis of structures. vibration. surfaces). At every step of the modeling process.

If it stops all running AxisVM programs stop.
.. AxisVM Version 8+ is shipped with a parallel port or USB Sentinel Super Pro dongle but earlier customers may have parallel port NetSentinel dongle. Insert the AxisVM CD in the CD-ROM drive of the AxisVM server.EXE from that folder. and select Run. Run NSRVGX..
F
Installation
To run AxisVM on any computer on the network NSRVGX must be running on the server.The system file is not suitable for running MS-DOS and Microsoft Windows applications. Insert the AxisVM CD into the CD drive. Select AxisVM 8 Setup and follow the instructions.
F
To run AxisVM on any computer on the network SuperPro Server must be running on the server.
F
If the setup program cannot be launched or the following message appears: AUTOEXEC. This type of network key requires at least a 7.NT . Two types of key are available: parallel port (LPT) keys and USB keys. If you have a network version you must install the network key. Windows NT must have Service Pack 3 or higher installed on the system to reach the key properly.eu /Support. Insert the AxisVM CD in the CD-ROM drive of the AxisVM server. You can download it: www. This server program handles the network key and communicates with the applications on the network. Installation
Software Protection The program is protected by a hardware key. 2.2.exe program on your AxisVM CD. b. Copy the contents of the folder [CD Drive]: \ Sentinel \ English \ server \ Disk1 \ Win32 to a folder of the server’s hard drive. CD contains the 7. Select Reinstall driver. 2.Service Pack for AxisVM 8+ • Click on the program icon with the Mouse right button after the installation of AxisVM program • • Choose the Properties menu item from the Quick Menu. click the Start button. Run [CD Drive]: \ Sentinel \ English \ Driver\ setup. a Windows system file must be missing. Run the Startup program and select Reinstall driver . Open the Startup. because certain operating systems try to recognize the plugged device and this process may interfere with the driver installation. This way you select the AxisVM server. If NSRVGX stops all running AxisVM programs stop. 3.
F
Plug the key only after installation is complete. Select the Compatibility tab on the appearing dialog and turn on the Run as administrator checkbox. Windows 98 requires a special driver to handle the USB port. The Startup program starts automatically if the autoplay option is enabled.14
AxisVM 8+Release 4
2. 4. For want of this driver the USB key does not operate.1 driver. If Autoplay is not enabled. If you encountered problems you can install this driver later from the CD..exe. Non-network drivers will be automatically installed. a.axisvm. Installation under Vista Operating System: • You need the latest Sentinel driver.
Standard Key Network Keys
First install the program then plug the key into the computer. NetSentinel dongle 1. Run [CD Drive]: \ Startup. In most cases AxisVM and the key are on different computers but to make the key available through the network the Sentinel driver must be installed on both computers.3 version of the driver. Connect the key to the parallel or USB port of one of the computers. Connect the key to the parallel port of one of the computers. This way you select the AxisVM server. AxisVM runs on Windows 98 / NT / 2000 / XP / Vista operating systems. Sentinel SuperPro dongle 1.exe to install Sentinel driver.

To turn it on choose the Settings\Preferences\Data Integrity dialog and check the Show welcome screen on strartup checkbox. Then you have to update your Windows by running [CD Drive]:\Comctl32\401comupd.0. 7. 3. The main steps of an analysis using AxisVM are: Creating the Model (Preprocessing) â Analysis Static Vibration Buckling (linear/nonlinear) (first/second-order) (linear initial) â Evaluating the Results (Postprocessing)
Steps of an analysis
Capacity
Practically.exe. Saving files in the file format of one of the previous versions (5.0. 6. Clearing the checkbox at the bottom turns the welcome screen off for the future. It is recommended to install the new version to a new folder. At startup a splash screen is displayed (see. and click the AxisVM8 icon. The setup program creates the AxisVM program group that includes the AxisVM application icon.. select Programs.0) is possible but this way the information specific to the newer versions will be lost. Saving files will use the latest format by default.4 About) then a welcome screen is shown where you can select a previous model or start a new one. the model size is limited by the amount of free space on your hard disk. You can specify the drive and the folders during the installation process. The restrictions on the model size and on the parameters of an analysis are as follows: Professional Entity Nodes Materials Elements Maximum Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited Unlimited
Truss Beam Rib Membrane Plate Shell Support Gap Spring Rigid Link
Load cases Load combinations Frequencies
.6.
F
Upgrading Converting earlier models
If you have an older version of Windows and Internet Explorer some toolbar icons may disappear. This way the previous version will remain available. Models created in a previous versions are recognized and converted automatically. Starting AxisVM Click the Start button.User’s Manual
15
By default the program and the example models will be installed on drive C: in C:\Program Files\AxisVM8 and C:\Program Files\AxisVM8\Examples folders.. AxisVM folder.

mesh the geometry into elements (assigning the properties and a mesh. Once the model is created it is ready for analysis. Please consult this User’s Manual every time you are using AxisVM. 5. In the second step you must specify material and element properties. In chapter 1 you can find the timely.3. Plane truss girder Plane frame Plate structure Membrane cantilever Seismic analysis
Loads
Understanding of these simple models will allow you to easily build more complex models. 3. 4.
. The end result will be a finite element model of the structure.2 Plane Frame Model There are three major steps in a modeling process: Geometry Elements The first step is to create the geometry model of the structure (in 2D or 3D). Chapter 2 contains general information about using AxisVM. to the wireframe model). and define the support conditions. new features of the version.and postprocessor menu structures. Getting Started
Step-by-step input schemes are presented in the Section 7. In other chapters the explanation follows the pre. In Chapter 7. the step-by-step modeling of a few typical structures are presented. 2.16
AxisVM 8+Release 4
Small Business Entity Nodes Materials Elements Only trusses Truss+Beam+Rib * Rib on the edge of a surface Membrane Plate Shell Any combination of membrane. It is recommended that you read the entire User’s Manual at least once while exploring AxisVM. In the third step you must apply different loads on the model. See Example 1 of Chapter 8 with a step-by-step input scheme in 7. The following types of structures are shown: 1. plate or shell Support Gap Spring Rigid Link Load cases Load combinations Frequencies (modal shapes) * If beams or/and ribs are in the structure
Maximum Unlimited Unlimited 500 250 1000 1500 1500 1500 1500 Unlimited Unlimited Unlimited Unlimited Unlimited 99 Unlimited 99
2.

4. transform Speed buttons in the bottom right provide the fastest access to certain switches (parts. These tools are accessible during any stage of work.4. move the cursor up to the menu bar. Please read these instructions carefully.13 Modify. move the pointer over it. See. The icons represent working tools in a pictorial form. and pick from menus and dialog boxes. Pet palettes appear when modifying geometry according to the type of the dragged entity (node. The cursor will change to a pointer. workplanes. The window shows the status of the model and results display. AxisVM screen After you start AxisVM a screen similar to the following picture appears:
Model name and location path Top menu bar
Pop-up
Color legend window
Cursor
Perspective Toolbar
Movable Icon bar
Property Editor
Status window Graphics area Pet palette Context sensitive help message Coordinate window
Speed buttons
The parts of the AxisVM screen are briefly described below. The window shows the color legend used in the display of the results. To select a menu bar item. symbols. or pointer. straight line. Its associated sub-menu will appear. select entities.)
Top menu bar
Active icon Icon bar
Coordinate window Color legend window Info window Context sensitive help Property Editor Pet palette Speed buttons
. sections. The icon bar and flyout toolbars are draggable and dockable. AxisVM User Interface
This section describes the working environment of the full AxisVM graphical user interface.8. and press the pick button to select the item.. The screen cursor is used to draw. Graphics area Graphics cursor The area on the screen where you create your model.. The window on the graphics area displaying the graphics cursor coordinates. it can appear as a pick-box. Your knowledge of the program increases the modeling speed and productivity. crosshairs with pick-box. Appears only in the post-processing session. Each item of the top menu bar has its own dropdown menu list.User’s Manual
17
2. numbering. The active icon represents the command that is currently selected. Provides a help message that depends on the topic under process. The Property Editor offers a simple way to change certain properties of the selected elements or loads. To use the top menu bar. arc). etc. Depending on the current state of AxisVM.

stress. AxisVM checks if AXS and AXE files belong to the same version of the model. Thus the program operates on a model that is an approximate of the actual structure. The shape of the cursor will change accordingly (See.
2. reinforcement. Moves the graphics cursor perpendicular to the current plane.axe file. You may assign only names that are valid Windows file names. Interrupts the command and/or returns to an upper menu level. That name will be used as a file name when it is saved.C. and will appear on the screen in one of the following forms: Crosshairs: Pointer: Crosshairs/zoom mode:
If you pick an entity when the cursor is in its default mode (info mode). Depending on the menu your cursor is on. Using the Cursor. These are termed command buttons. To each model you must assign a name. The model consists of all data that you specify using AxisVM. To select an entity. Activates the main menu Moves the focus from control to control in a dialog. internal force. you may get the properties of the following entities: Geometry Elements Loads Mesh Static Vibration Buckling R. [End] [Esc] or 8 right button [Enter]+[Space] 8 left button [Alt] [Tab] node (point) coordinates. 4. the Keyboard. cu stom α or α +n·90°.. move the cursor over it and click the left mouse button.8 [Home] [End] [Ctrl]+ [Home]. influence line ordinate mode shape ordinate mode shape ordinate specific reinforcement values k results and resistances
You can also use the keyboard to move the cursor: Moves the graphics cursor in the current plane.1 Cursor Identification). 8 [Shift]+ [↑][↓][←][→]. Moves the graphics cursor perpendicular to the current plane with a step size enlarged/reduced by a factor set in the Settings dialog box. Design Steel Design The keyboard Arrow keys. The model’s data are stored in two files: the input data in the filename. support element load. executes a command.7. the graphics cursor symbol tracks the movement on the screen. line length finite element. reference. and selects entities.
. degree-of-freedom. 8 [Ctrl] + Arrow keys.. Moves the graphics cursor in the current plane on a line of angle n·∆α .axs and the results in the filename.18
AxisVM 8+Release 4
The model
With AxisVM you can create and analyze finite element models of civil engineering structures. an icon or menu item. the properties of that entity will be displayed as a tool tip. Selects an item from a menu. Moves the graphics cursor in the current plane with a step size enlarged/reduced by a factor set in the Settings dialog box.5. the Mouse
Graphics cursor As you move your mouse. nodal mass meshing parameters displacement.

The program saves the latest position and displays the dialog on the same position next time. All the tables AxisVM creates are available through the Table Browser dialog box by clicking its button or pressing [F12]. displayed) part is listed by default. If you use Table Browser while working in the pre-processor. by pressing the right mouse button a quick menu appears in accord with the current command in use.9.
[F12]
F
Only the data of the current selection (if any) or of the active (i.
.7. While working in the post-processor. You can change the position of all dialog windows. the model results are also displayed. The tables operate in the same way independent of the content displayed. The model data to be displayed in the Table Browser can be selected from the tree structure in the left side of the browser.20
AxisVM 8+Release 4
Hot keys in the Report Maker [Ctrl]+[T] [Ctrl]+ [Alt]+[B] [Ctrl]+[W] [F3] [Ctrl]+[P] [Ctrl]+[Del] Insert text Insert Page Break Export to RTF file Report Preview Print Delete
2.8. Dialog Boxes
After selecting a function usually a dialog box appears on the screen. These dialog boxes can be used the same way as any other Windows dialog. input model data is displayed only.e. Quick Menu
8 right button
When the cursor is over the graphics area.
2.
Selection Geometry / Elements / Loads Results
2. The dialog font can be changed by selecting the Settings\Preferences\Fonts dialog and clicking the font sample label Dialog boxes. Table Browser
AxisVM uses tables to display numerical information on the screen allowing changes in formatting.

Clicking a fixed (topmost) cell of a column selects the column. result tables and libraries in a hierarchy and can also be used as a model overview. Clicking an editable cell moves the edit focus to that cell. Displays the previous page of rows. Displays the next page of rows. Moves the focus to the previous (to the left) page of columns (only in tables where more columns can be displayed at the same time). Ends the current editing in the edit box storing the data entered and moves the edit box a column to the right or to the first column of the next row. to the left and to the right. Moves the focus to the first cell of the first row Moves the focus to the last cell of the last row. and scrolls the table along the rows or columns. You can also select cells by dragging the mouse. Moves the focus to the first cell of the row. Set Common Value below
Arrow keys
8 left button
[Home] [End] [Ctrl]+[Home] [Ctrl]+[End] [Page Up] [Page Down] [Ctrl]+ [→] [Ctrl]+ [←] [Enter] [Esc]
8 right button
[Shift]
. It can be viewed in its entirety using the scroll bars and/or using the keyboard as follows: Moves the edit focus up and down..User’s Manual
21
The tree view on the left lists element / load data.
Add New Row Cross-Section Editor Library Copy Delete Paste Format Print Fit Filter
Add to Report
Using the table
A table can contain more rows and/or columns than can be displayed at the same time. Clicking the top left cell selects the entire table. Moves the focus to the last cell of the row.. Moves the focus to the next (to the right) page of columns (only in tables where more columns can be displayed at the same time). While the [Shift] key is down all direction keys will select cells instead of moving the edit focus. Selected cells can be copied to clipboard as a table. If selection is within an editable column you can set a common value for the selected cells. Clicking a fixed (leftmost) cell of a row selects the row. See. Aborts the current editing in the edit box.

htm.. with the page header and comment row previously set with the File/Header menu command. You can delete a user defined table. You can import this file into Microsoft Word or any other word processor which can import RTF files.dbf. You can store cross sections of any type in these tables. Exports the current table into a TXT (ASCII) file name. [Ctrl]+ [L] Import DBase File
Loads cross-sectional or material data from a library.dbf into the current table.10. Type of the table determines only the position of the table in the Cross-section Library. Exports the current table into a Dbase file name. cross.
Save As DBase File
Save As HTML
Save As TXT
Save As RTF
Exports the current table into an RTF file name. [Ctrl]+ [P] Exit [Alt]+ [F4] Edit
. Some formatting information of the columns will be lost. You can modify properties (table’s name.rtf using the current template file. Exports the current table into an HTML file name. Exits the table in the same way as the Cancel button (the changes are not saved). This file can be imported as a table into Word or can be opened in web browser applications. The table created will be placed together with the cross-sections of the same type.sec. 2.section type) of a user defined table.22
AxisVM 8+Release 4
File
Browse Library .1 Report Creates a new cross-section data file name. The program checks the values of the fields and sends an error message if an incompatible value is found.txt.
New Cross-Section Table
Cross-SectionTable Properties Delete Cross Sectin Table Print . You can also save the current content of the table in a custom library. Imports a DBase file name. The field names are generated based on the names of the columns. The fields will be of text type. Prints all the information displayed in the table to the selected printer or to a file.. See.

Available from the Table Browser Menu / Edit / Set Common Value. If entire rows were cut or copied and the table allows inserting new rows you can also add clipboard data to the end of the table instead of overwriting the existing rows. The display format is set according to the settings in the Units/Settings dialogue window (see. Jumps to a specified row in the table.
. allowing the modification of a custom cross-section previously created with the graphics Cross-Section Editor..
Set Common Value
Go to [F5] Format Defining data
Column Formats
You can specify whether a column is visible or not.key is deactivated while entering these kind of values. Copies selected cells to the Clipboard as a table.
Pastes table cells from the Clipboard overwriting cell values. Many cells require the entry of a numeric value. Deletes the selected rows. When entering real numbers you can use the following characters: +-01234567890E and the standard Windows decimal separator specified in Start / Settings / Control Panel / Regional Settings / Number / Decimal symbol field.User’s Manual
23
New [Ctrl]+ [Insert] Delete [Ctrl]+ [Del] Select Table [Ctrl]+ [A] Design New Custom Crosssection [Ctrl]+[G] Modify Custom Cross-section [Ctrl]+[M] Automatic crosssection shape update Delete unused cross-sections Copy [Ctrl]+ [C] Paste [Ctrl]+ [V]
Adds a new row to the list.
If this function is on changing section parameters in the table leads to the recalculation of geometry and cross-section parameters.3. Starts the graphics Cross-Section Editor. allowing the input of a new custom cross-section.. and allows you to fill all the editable cells with data in a fixed order from left to right. Example: you can set the Z coordinate of all nodes to the same value making the model absolutely flat. Sets a common value for the selected cells within a column.
[Ctrl]+ [Alt]+ [F]
Format Defaults [Ctrl]+ [D]
Restores the default format of the entire table (column visibility and decimals).
Starts the graphics Cross-Section Editor.
Selects the entire table. In some cases you cannot enter a negative number so the . Clicking the top left cell does the same. Unused cross-sections will be deleted from the table. If an integer value is required you cannot use the decimal separator and E. by setting the check boxes of the corresponding columns.6 Units and Formats).3. If any of the values is unacceptable Paste aborts.

See in detail: 6.
Result query
Result Display Options [Ctrl]+[R] Results On/Off [Ctrl]+[T] Extremes On/Off [Ctrl]+[E] Order of load cases. Load Groups
Property Filtering [CTRL]+[Q]
Property filtering helps you to select which elements to include in the table. Adds the current table to the current report. If the current table is a result table and is set to display extremes only all sub-tables will display extremes only. Report
Current report Add table to report [F9] Report Maker [F10]
You can set the current report....4 Result Tables Display of results can be turned on / off.
. In case of result query new items appear on the Format menu and the Toolbar. MODEL or Loads) all tables under that node will be added. See. See.24
AxisVM 8+Release 4
Show used crosssections in boldface
In case of Cross-section Table it helps the orientation..10. The cross-names which are signed by bold letter will remain in the table if the Delete Unused Cross-sections switch is turned on.
You can control finding the extremes for result components and set to show results (Result) and/or just the extremes (Extremes).10 Report Maker... The display order of load cases can be customized..10 Report Maker.
Display of extremes can be turned on / off. If the selected node in the treeview has sub-nodes (e.2..1 Load Cases. Opens Report Maker. See.g. 2. Tables will be added to this report. 4. See… Edit menu item.1.

Result tables also display the extremes (minimum and maximum values) of the data if you select this option in the Display Options dialog when you enter Table Browser.
F
2. Report Maker can handle several different reports for the same project. Report Maker
[F10] Report Maker is a tool to compile a full report of a project using report items (tables/drawings/pictures created by AxisVM and user-defined text blocks). Displays info about the table browser operation.10.axs) and can be printed or saved as a Rich Text Format (RTF) file. The properties of the selected report item are shown on the right side of the window.
. RTF files can be processed by other programs (e.g. Saves the data and closes the table. Tables exported from Table Browser are automatically updated if the model has been changed or some of its parts were deleted. Closes the table without saving the data. Microsoft Word). The structure of reports is displayed in a tree view on the left. Displaying both the individual values and the extremes is the default setting.User’s Manual
25
Help
About Table About Table Browser OK Cancel
Displays info about the table. Reports are stored in the model file (*.

10. See. In printed reports Report Maker automatically builds a table of contents and inserts it to the beginning of the report.8 Save to Drawings Library. JPG. Unlike the pictures in the Gallery these drawings are not graphics files.5...2. WMF. 3. 3. to make changes.
Drawings Library
By clicking the Drawings Library tab you can browse the saved drawings and add the selected ones to the report. its comment text. EMF) located in a folder named Images_modelname and add the selected ones to the report. 2. alignment and caption can be set.. See in detail. If a text block is selected the text is shown on the right. Display of title.. column titles and other properties are shown.. Pictures are listed only if they have a caption.7 Drawings Library... If a picture or drawing is selected it is shown on the right. Its size. By clicking the Gallery tab you can browse the saved pictures (BMP. This folder is automatically created as a subfolder of the model folder. See in detail.
Gallery
. comment and columns can be turned on and off. Click the button Edit text. Text blocks are listed only if they were formatted using one of the Heading styles in the Text Editor.26
AxisVM 8+Release 4
Table Text Picture or Drawing
If a table is selected. This way drawings will be automatically updated if we change and recalculate the model. but view settings stored to recreate the drawing at any time.4 Gallery You can save the current drawing on screen or the result tables in design modules with the function of Edit\ Saving drawings and design result tables in main menu. 3. Tables are listed according to their titles..5.8 Saving drawings and design result tables One or more selected pictures in the Gallery can be inserted into a report by selecting menu item Gallery/Add pictures to the report or clicking the arrow button above the Gallery or by drag and drop.

Pictures used in the report are not deleted from Gallery. Character and paragraph formatting of text blocks will be exported. [Ctrl]+[Del] Rename Save As TXT Export as RTF
Deletes the current report (i. To print the RTF report on a different machine make sure that picture files are also copied to a subfolder Images_modelname. Drawings or pictures are not included. Table titles are formatted with Heading 3 style so it is easy to build a table of contents automatically using Microsoft Word. Exports the report into a ASCII text file. Gridlines of exported tables can also be turned on/off.rtf using the current template.User’s Manual
27
2. [End] = last page. A dialog to set printing parameters and print a report.
Delete entire report [Del]. Link to BMP. Saves the report as name. [PgDown] = next page. Read the text of the template file carefully before changing it. The only exception is the character color. Embedded WMF: Drawings are embedded into the file.
RTF Options
Report preview [F3] Print [Ctrl]+[P] Exit
Displays a print preview dialog.
Gives a new name to an existing report. It is necessary because pictures are only linked and not saved into the RTF document.1. JPG: This option keeps the RTF file smaller as drawings are stored in external files. The options are the same as the table printing options. Tables will be exported as RTF tables.
. When changing a template you can create your own cover sheet and header/footer for the report.10. You can set the zoom factor between 10% and 500% (Page Width and Full Page is also an option). AxisVM saves reports to RTF files using a template (the default one is Template.e. Quits the Report Maker. If you save the file to a folder different from the model folder all picture files used in the report are copied to an automatically created subfolder Images_modelname. Click the buttons or use the keyboard to move backward and forward between pages ([Home] = first page. In Insert / Index and Tables or Insert / Reference / Index and Tables select the Table Of Contents tab of the dialog. the report which contains the selected item). [PgUp] = previous page. set Formats to From template and Show levels to at least 3. You can use other templates as well. Drawings appear only if pictures are located in an Images_modelname subfolder relative to the folder of the RTF file. Format of drawings in RTF file can also be set. Report
New report
Creates a new report. It improves portability but can result in huge file size.rtf in the program folder). Report names can be 32 characters long.

result components. or if you want to see result components listed within a load case or load cases listed within a result component. Edit
Some of the functions in the Edit menu are also available in the popup menu after clicking right mouse button on a report item. Report Builder creates complete structured reports based on several filter options set on the Filter tab. Executes the command which was undone. The report sent to the report maker will contain the checked items only. Undo Redo Report Builder Undoes the effect of the previous command.28
AxisVM 8+Release 4
2.2. The number of expanded levels (1-7) of the report tree on the right can be set with the level-adjustment bar. Load cases. If we imported an architectural model it is also possible to filter for architectural objects and ask for separate tables for each architectural object.10. Each report item can be turned on/off individually. You can choose if you want to see different element types listed within a part or different parts listed within an element type. The rules of creating reports can be set on the Preferences tab.
Filter
. The tree on the right side shows the report built using the criteria set in the left. parts. element and load types can be selected and set the display of extremes or results in the tables.

Every report item of the current report will be selected. The number of expanded levels (1-7) of the report tree can be set with the level-adjustment bar. The formatted text will be inserted after the selected report item. If the current selection in the tree is a report it deletes the entire report.User’s Manual
29
Preferences
Insert folder
Inserts a new folder into the tree. Deletes the selected report item (text block. Determines which types of report items can be selected (report. table. table. If you turn this checkbox on and select a folder all subitems will be selected automatically. drawing. The current folder name appears on the right side under the folder icon. page break. page break). Deselects all selected items in the documentation.
Move to / Copy to Selection filter Select subitems automatically Deselect all Select all items of the current report Delete [Del].
Deletes all items from the current report but does not delete the report itself. text. picture.
Moves up/down the selected report item by one. folder). [Ctrl]+[Del] Delete all report items
Moves / copies the selected report item to the end of another report.
Insert text into report [Ctrl]+[T] Page break [Ctrl]+[Alt]+[B] Move up/down selected report item
Inserts a page break after the selected report item.
. below the current item. Starts a built-in Text Editor to create a new text block. picture.

2. Files are permanently deleted... . If checked pictures are sorted in descending order. . Place of insertion is determined by the selected item of the report tree.
Delete pictures from Gallery
Deletes selected pictures from the Gallery. Gallery
Add pictures to the report Copy pictures to Gallery
Inserts selected pictures into the current report.1 Report Creates a new report based on several filter options. 2.10. button on the Drawings
Format of drawings in RTF file.JPG) and Windows Metafiles (.WMF.3..EMF) to the folder Images_modelname..WMF) or by date.. Otherwise pictures are sorted in ascending order.10. . 2.2 Edit
[Ctrl]+[T]
. 2.1 Report Inserts a folder under the current folder or after the current list item.1 Report
2. 2..10. See.10. See. .10. See..
2.5.4.JPG.. . See. The Report Toolbar
Creates a new report.EMF. Effect of this function is the same as that of the Library tab...
See.BMP.10.10.BMP..2 Edit Inserts a formatted text after the selected report item..
Delete unused pictures Sort by name / type / date Reverse order
Deletes pictures which are not used in the reports. You can copy bitmaps (. Gallery sorts pictures by filename / by type (.30
AxisVM 8+Release 4
2. Drawings
Add drawings to the report
Inserts the selected drawing(s) from the Drawings Library into the selected report.10.

2.10.6. Gallery and Drawings Library Toolbars
You can perform certain tasks faster using these small toolbars. Deletes selected pictures or drawings from the Gallery/Drawings Library. Inserts selected pictures or drawings into the current report. Place of the insertation is determined by the selected item in the report tree. Copies pictures from other locations to the Gallery. This function is not available on the Drawings Library tab.

2.10.7. Text Editor
After selecting Insert text to report a formatted text can be created in a simple WordPad-like text processor. File Open [Ctrl]+[O] The main purpose of this function is to load a Rich Text file written in Text Editor. If you open an RTF file created in another word processor it may contain special commands (e.g. tables, paragraph borders, Unicode characters) which are not supported this simple editor. As a result you may get a series of rtf control commands instead of formatted text. Saves the text into an RTF file. Quits Text Editor. Undoes / redoes the last editing action.

You can search for any text in the document. You can search from the beginning or from the current position. You can search whole words only and turn on and off case sensitivity. If a match was found you can get the next match with this function. Selects the entire text.

Applies bold formatting to the selected text.

Applies italic formatting to the selected text.

Applies underline formatting to the selected text.

Sets the character color of the selection.

Justifies the selected paragraphs to the left.

Justifies the selected paragraphs to the centerline.

Justifies the selected paragraphs to the right.

Places bullets before the selected paragraphs.

2.11. Redraw
Pressing this button you can make the screen redraw.

2.12. Layer Manager
See in detail... 3.3.3 Layer Manager

2.13. Drawings Library
See in detail... 3.5.7 Drawings Library.

2.14. Save to Drawings Library
See in detail... 3.5.8 Save to Drawings Library.

User’s Manual

33

2.15. The Icon bar

Selection Zoom Views Display mode Transformation Work planes Guideline Geometry Tools Dimensioning/Labeling Parts Sections Searching Display option Options Model info If you choose Workplanes, Dimensioning - Model info a dialog will appear. Dragging and docking the Icon bar and the flyout toolbars The left-side icon bar and any flyout toolbar can be dragged and docked. Dragging and docking of the Icon bar If you move the mouse over the handle of the Icon bar (on its top edge), the cursor will change its shape (moving). You can drag the Icon bar to any position on the screen. If you drag the Icon bar out of the working area through its top or bottom edge the Icon bar becomes horiozontal. If you drag it to the left or right edge it becomes vertical. If the Icon bar is horizontal you can dock it at the top or at the bottom. You can change the position and the order of docked toolbars by dragging. In the Cross-Section Editor and in Beam and Coumn Reinforcement dialogs the Icon bar cannot be docked. Closing a floating Icon bar restores its original position docked on the left. Dragging and docking of flyout toolbars You can also separate flyout toolbars from the Icon bar by dragging their handle. Closing or dragging them back to the Icon bar restores their original position. Floating flyout toolbars can be docked at the top or at the bottom.

F

The Icon bar and the flyout toolbars can be restored to their original position by selecting Settings\Toolbars to default position from the menu

Lets you select a set of entities (nodes (points), lines, finite elements and loads) for processing. When you execute commands you can use the Selection icon to specify the entity set to which to apply the command to. If the Parts check box (See section 2.15.10 Parts) is enabled the selection will refer only to the active (visible) parts. You can change the view settings or continue selection in another window pane during the selection process. These allow you to select elements in the most convenient view. The selected entities are displayed in magenta in the graphics area. The selection process is considered finished when the OK button is pressed. Selection methods with selection frame: - dragging the selection frame from left to right selects elements entirely within the frame - dragging the selection frame from right to left selects elements which are not entirely outside the frame Select Deselect Invert All Previous Selection of parts Filter Adds the currently selected entities to the set of selected entities. Removes the currently selected entities from the set of selected entities. Inverts the currently selected entities’ selection status. Applies the current selection mode (add, remove, or invert) to all filtered entities. Restores the previous selection set. Clicking the button and a part from the list will select elements of the chosen part. Lets you specify filtering criteria to be used during selection. Check element types to select. Property filtering lets you apply further criteria (beam length, cross-section, material, surface thickness, reference).

User’s Manual

35

Method

Selects entities using different methods (selection shapes). Rectangular, skewed rectangular, sectorial or ring selection shapes are available. In the followings examples of the application of various selection shapes are provided: Selection: Rectangular Result:

Skewed rectang.

Polyline

Sectorial

Annular

Intersected lines

OK Cancel

Ends the selection, retaining the selected set for use. Ends the selection, discarding the selected set. If an entity is hidden by another entity you cannot select it by simply clicking on it. In such a case, you have to change view to select it.

F

36

AxisVM 8+Release 4

$

The selected nodes are marked with a surrounding magenta rectangle. Sometimes it is necessary to double-select nodes. In this case these nodes are marked with an additional blue rectangle surrounding them. Selections can also be made, without using the Selection Icon Bar. Pressing and holding the [Shift] button while selecting with the 8 will add entities to the selection and pressing and holding the [Ctrl] button while selecting with the 8 will remove entities from the selection. Double selections can be made by pressing and holding the [Alt] button while double clicking on the entities with the 8.

F

During the selection we can modify the apperiance of the structure, we can switch over an other view or perspective observation.

2.15.2. Zoom
Displays the zoom icon bar.

Zoom in

Displays an area of the model drawing specified by two points (two opposite corners) on the graphics area defining a rectangular zoom region. As a result, the apparent size of the model displayed in the graphics area increases. Displays the model drawing from the graphics area on the area specified by two points (two opposite corners) defining a rectangular zoom region. As a result, the apparent size of the model displayed in the graphics area decreases.

Zoom out

Zoom to fit

Scales the drawing of the model to fit the graphics area, so you can view the entire model. Moves the drawing. Press and hold the left button of the 8 while moving the mouse, until the desired position of the drawing is obtained on the screen. Quick Drag: You can use the mid mouse button to drag the model drawing at any time (without the the Pan icon). 1. 2. Click the Pan icon. Drag the model to its new position. This cursor shape indicates that you can pan the model.

Pan

$

15. Rotation around an axis perpendicular to the screen. Perspective Toolbar
Axonometry Perspective Rotate about the perpendicular axis Rotate about the vertical axis Rotate about the horizontal axis
X-Z view X-Y view Z-Y view
Rotate (activates the pet palette) Observation distance New perspective view Perspective view list Delete active perspective
Sets the parameters of the perspective display. During the rotation the following pet palette appears at the lower part of the screen: Rotation methods in the order of icons: Free rotation around the horizontal axis of the screen and the global Z axis. Rotation angles can be set with a precision of 0. Type a name into the combo and click on the icon on the left of the combo to save the settings.
.1 degrees. To delete a perspective setting choose it from the dropdown list and click on the Delete icon on the right side of the combo. Rotation around the vertical axis of the screen. Rotation around the global Z axis. Undoes / redoes the action of up to 50 view commands. The proper view can be set by rotating the model drawing around the three axes.
2.3. Rotation around the horizontal axis of the screen.
$
Undo view / Redo view
This cursor shape indicates that you can rotate the model.User’s Manual
37
Rotate
After clicking this icon you can rotate the model around the centre of the encapsulating block of the model by dragging. You can assign a name to each setting that you want to save for later use. Displays the projection of the model on the Y-Z plane (side view). Displays the projection of the model on the X-Y plane (top view). Views
Displays the projection of the model on the X-Z plane (front view). After clicking on the rotate icon a pet palette appears as described earlier (Zoom\Rotate). and by setting the observation distance. Observation distance Rotation Observation distance is the distance between the viewpoint and the centre of the encapsulating block of the model.

perspective
Displays three projection views and the perspective view of the model. These workplanes follow the local system of a truss.38
AxisVM 8+Release 4
Views. and allows you select the view that you want to display. beam. Using multi-window mode a different workplane can be set for each window. Useful when drawing stories of a building. rib or domain. These workplanes are defined by an origin and two vectors for the local x and y axes. After checking Hide elements not in the workplane only those elements are displayed that are in the workplane. After checking Show elements out of workplane grayed elements out of the workplane appears grayed. The origin is the first point of the element.15. Workplanes are also available from the main menu by selecting View \ Workplanes or from the popup menu by selecting Workplanes. Global Y-Z workplanes General workplanes
All drawing/editing functions are available in workplane mode. Clicking the workplane speed button the workplane can be selected from a list. Consider a hole for a skylight on an oblique plane of a roof.4.
F
Global X-Y.
Display options
A workplane can be displayed in the global coordinate system or in its local system. local x and y axes are parallel to the local x and y axes of the local system of the element. Deleting the finite element you delete the workplane as well. The plane of the roof can act as a workplane so drawing can be performed in two dimensions. Workplanes
Workplanes (user coordinate systems) makes it easier to draw on oblique planes. These workplanes are parallel with a global coordinate plane so their position is defined by a single coordinate.
Smart workplanes
F
Changing the local system of the finite element the workplane is also changing.
. Global X-Z. In case of workplanes altitudinal coordinate means the distance along the axis normal to the workplane. Click the view you want to select.
2.

dZ (by dX/N. You can choose one of the following options: None: No nodes will be connected. Lets you define workplane parameters (origin or axes) graphically. dY. Copy dimension lines: The dimension lines will be copied only if the nodes to which they are assigned are selected. The number of copies depends on how many copies will fit into the length defined by the translation vector dX.
2. Deletes user defined workplanes.User’s Manual
39
Changing workplane parameters Delete Pick Up >>
If you select a workplane from the tree. dY. Consecutive: makes N consecutive copies of the selected entities by different distances dX.1. Geometric tranformations on objects
2. All: All nodes to be copied will be connected. dY.5. dY/N.
Translation options
Incremental: makes N copies of the selected entities by the distance dX. Distribute: makes N copies of the selected entities along the distance dX. and the number of copies (N).5.15. Copy nodal masses: You can specify the nodal masses to the geometric entities to be copied as well. by translation along a vector.
F
Loads can be copied separately (without the elements).
. dZ). or moves the selected geometric entities or loads. its parameters are displayed. dZ. dY. You must specify the translation vector (dX. dZ. dZ/N increments). Move: moves the selected entities by the distance dX. These nodes will be connected. dZ. Editing them and clicking the OK button or selecting another workplane will change the parameters of the selected workplane. dZ.
Nodes to connect
You can select nodes that will be connected by lines to its corresponding copies. Double selected: Holding the [Alt] key pressed you can double select nodes. Translate
Translate Makes multiple copies of. Spread by distance: makes copies of the selected entities spread by distance d in the direction of the translation vector.15. Copy loads: You can specify the loads assigned to the geometric entities to be copied as well. dY.
Switches Copy options
Copy elements: You can specify the finite elements assigned to the geometric entities to be copied as well. dY.

2. Selected loads can be copied or moved to another load case if load case is changed to the target load case during the operation. 4. support conditions. by rotation around a center.
Rotation options
Incremental: makes N copies of the selected entities by the cursor angle. You can use any existing point when you have to specify the translation vector. and then make copies of them. 3. The translation consists of the following steps: 1. Move: moves the selected entities by the cursor angle. In X-Y. Rotation
Rotate Makes multiple copies of. Consecutive: makes N consecutive copies of the selected entities at different cursor angles.2. the number of copies (N) and an additional translation h along the rotation axis (each copy will be shifted by this distance).
. The number of copies depends on how many copies will fit into the cursor angle. and dimension lines). Click the rotation center (OX. In perspective view rotation axis is always the Z axis. you should first create these (including the definition of finite elements. 6. Distribute: makes N copies of the selected entities by cursor angle/N increments. Parameters depend on the method: rotation angle α. You can specify the method of rotation. With this option checked the transformations will be performed on the objects of the DXF layer as well.15.40
AxisVM 8+Release 4
With guidelines With DXF layer Visible layers only Steps of translating
All rulers will also be moved (useful when moving the entire model). With this option checked only the visible layers will be transformed. the rotation arc start point and draw the cursor angle. Click on the Translate icon Select the entities or loads to be copied Click OK on the Selection Window (or Cancel to interrupt the selection and translation commands) Select your options from within the Translate Window. OZ).
2.5. OY. loads. X-Z or Y-Z views the rotation axis is normal to the current view plane. Spread by angle: makes copies of the selected entities spread by a given angle α specified in the dialog. 5. Click OK Specify the translation vector by its start and end point
The command can be applied in the 2-3-1-4-5-6 sequence as well. or moves the selected geometric entities or loads.
F
If you have repetitive parts in your model.

Mirror options
Nodes to connect Switches
See. 2.15. Incremental: makes N scaled copies of the selected entities by repeating the scaling N times...5.15..5. 2. a point of reference and its new position after scaling (coordinate ratios will determine the scaling factors).5.1 Translate In perspective view. Resize: redefines the selected entities by scaling. by mirroring.1 Translate See..1 Translate See.1 Translate In perspective view.15.. 2.5..5. Consecutive: makes differently scaled copies of the selected entities in consecutive steps.. Distribute: distributes N scaled copies of the selected entities between the original and the scaled image.15.4. The symmetry plane is always parallel to a global axis depending on what view you are in. Mirror
Mirror Makes a copy of. Move: moves the selected entities across the mirror plane. or moves the selected geometric entities. See.15..15.15.e.5.5.. a point on a line). In perspective view.. by scaling from a center. 2. 2. start point and endpoint can be specified only using existing points or other identified 3D locations (i. You must specify the scaling center. 2.3. Multiple: makes consecutive copies of the selected entities over different mirror planes. Specify two points of the symmetry plane. Copy: reflects a copy of the selected entities over the mirror plane.5. cursor angle is determined by the global X and Y coordinates only.1 Translate See.User’s Manual
41
Nodes to connect Switches
See.1 Translate
Scale options
Nodes to connect Switches
. the centerpoint..15. or moves the selected geometric entities or loads. the mirroring is possible only across a plane parallel with the global Z axis..
2.
2. Scale
Scale Makes multiple copies of.

The elements colors are displayed corresponding to colors assigned to their materials. Vertical line elements are considered to be columns. In this mode the axis of the line elements and the mid-plane of the surface elements are displayed. horizontal domains as floors.. vertical domains as walls. Hidden : Displays a wireframe model drawing with the hidden lines removed. horizontal ones are handled as beams.15. The line elements are displayed with their actual cross-section and the surface elements with their actual thickness. Rendered view is smoother and shows the details of thin-walled cross-sections. Display Mode
Wireframe : Displays a wireframe model drawing..42
AxisVM 8+Release 4
2. In View / Rendering options.
Opaque
Transparent
.6. Element types are determined by geometry.
Rendered : Displays a rendered model drawing. transparency of element types can be set.

The cursor identifies the guidelines.7 Editing Tools
$
The guidelines are displayed as blue dashed lines.User’s Manual
43
2. You can change the position of a guideline with the mouse by dragging it to a new position. This way an arbitrary grid can be created. Places an oblique guideline at the current position of the cursor. See. Guidelines can be defined in the global coordinate system. the following dialog is displayed:
guideline
b a
a: is the angle of the guideline’s projection on the X-Y plane and the X axis.. The display of the guidelines can be enabled or disabled in the Display Options menu (or icon) in the Switches section.7. b: is the angle of the guideline and its projection on the X-Y plane.
Places a vertical guideline at the current position of the cursor. 4. You can remove (delete) a guideline by dragging it off the graphics area. Clicking with the mouse on a guideline or selecting Settings/Guidelines Setup command from the main menu.15.. Places a horizontal guideline at the current position of the cursor.
. Places a pair of orthogonal oblique guidelines at the current position of the cursor. Guidelines can be entered numerically by coordinates. Places a vertical and a horizontal guideline at the current position of the cursor. In perspective view all the guidelines are displayed but only oblique guidelines can be placed. Guidelines
Helps in editing the geometry of the model. intersections can be determined and distances can be set.

15. These icons can be conveniently used while editing the geometry of the model or defining section planes. Bisector will determine the direction of the line. Click on the Dimensions icon to display the Dimension Toolbar. The cursor will move perpendicular or parallel to this baseline.44
AxisVM 8+Release 4
2. The cursor will move perpendicular to the plane. as well as angle. level and elevation marks. Line towards a midpoint Using of icon: begin to draw a line then click startpont and endpoint of another line. Click on the left-bottom icon of the Dimension Toolbar to set the parameters of the selected tool. arc length.9. Perpendicular to a plane Begin to draw a line. labels or result values. Bisector Using of icon: begin to draw a line then click the two legs of an angle. That will allow you to select the proper dimension tool.15.
2.
You can change the position of dimension lines or labels at any time by dragging them to their new position. The plane can also be defined by clicking three points.8. Dimensions Lines.
. Click the Perpendicular or Parallel icon then click an existing line or click two points to define the direction. arc radius. Click the Perpendicular to a plane icon then click the domain defining the plane. Symbols and Labels
This group of functions lets you assign associative orthogonal and aligned dimension lines or strings of dimension lines to the three dimensional model. Perpendicular Parallel
Baseline Baseline
Begin to draw a line. If the dimension lines were associated with the model their position and dimension will be continuously updated as you modify the geometry of the model. Midpoint will determine the direction. Geometry Tools
The icons of Geometry Tools allow you to lock the direction of drawing a line.

All intermediate dimension lines will be created automatically. dY. A string of dimension lines can be selected at once if you click on one of them while depressing the Shift key. To insert a string of dimension lines. As a result this dimension line will be removed from the group (it can be moved individually). A string of dimension lines can also be created by turning on the smart dimension lines.g. In this case you have to select the direction dX. Orthogonal and Aligned Dimension Line Settings
. it will always behave in an associative way (e.1. will move with the model when the model is changed or resized or moved). 3. Click the left mouse button to set the final position of the dimension line. To change the position of a group segment individually select it using the selection rectangle and drag it to its new position.9.User’s Manual
45
2. It allows you to move it as a group.15.
Orthogonal Dimension Lines Associative orthogonal dimension lines or strings of dimension lines. The position of the dimension line depends on the direction in which you moved the mouse. or Z axes can be assigned to the model by following the next steps: 1. you have to select only the end points of the string. parallel with the global X.
Smart dimension lines
An example of smart dimension lines If the dimension line is assigned to the points of a model. 2. click on the points in the corresponding order or on the lines if any. or dZ from the toolbar. Y. Move the mouse. There is one exception: when the segment is not parallel with any global plane and the editing is in the perspective view. If you enable this function by pressing the button. Click on dimension line start point and on the end point. If these points are connected by a line you can just click on the line. Steps 2 and 3 are the same as for the individual dimension lines. assuming that the intermediate points were not generated by a domain mesh command.

a Dimension layer will be automatically created.
Display unit of measurement Units and Formats. See.46
AxisVM 8+Release 4
Tick mark Color
Lets you set the tick marks of the dimension lines. The dimension lines. Lets you restore the default setting. You can get the color from the active layer. By clicking the Units and formats button the number format can be set in the Dimensions section of the Settings / Units and Formats dialog box.. Measured value Allows you to place the measured value on the dimension line. Auto horizontal/vertical.. You can select from nine predefined symbols. Always vertical. You can turn on/off the display of extension lines. Lets you set the color of dimension lines individually. 3.3 Layer Manager Text Parameters
Sizes Dimension style/ Extension style Label orientation
Use defaults Apply font to all symbols Save as default setting Apply to all dimension lines Layers
Allows to you to define the settings of the text on the dimension lines. Apply the same font to every dimension line.. Lets you set the drawing parameters of the dimension line. Lets you save the current setting as default setting.. To change the current font parameters click the button below the Units and formats. Lets you set the orientation of the text labels of the dimension lines (Always horizontal. Applies the current setting to all existing orthogonal or aligned dimension lines to ensure a uniform look. If there are no layers defined when you start defining dimension lines. You can choose a predefined value or get it from the active layer. and texts are placed on the Dimensions layer by default but you can change it any time. Display of the unit of measured value. Lets you select/define/set layers where the dimension lines will be placed. using the current prefix and suffix settings. Lets you to set the type and thickness of a dimension or extension line. marks. or Aligned to dimension line) inside or outside the dimension line.3. button.
..

If the points are connected by a line you can just click on the line. dZ.2. or Z from the toolbar. dY. For aligned dimension lines the automatic prefix is always dL= or DL=. 4. The plane of the parallel dimension line is determined automatically. Y.. Sets the suffix used with the text on the dimension lines.9.9.3. You can choose from the following options: Auto (dX. dL = [depending on the direction]) Auto (DX.15.9. DY. There is one exception: when the segment is not parallel with any global plane and the editing is in the perspective view.
Angle Dimension Associative angle dimensions. The plane of the section line will be defined by the segment and the selected global axis. An example of associative dimension lines (orthogonal and aligned):
Before Scale command
After Scale command
2.15.. Click the left mouse button to set the angle dimension in its final position. can be assigned to the model in the following steps: 1.
. Sets the dimension line settings (See. 3. DZ. If the points are connected by a line you can just click on the line. 2.15...1 Orthogonal Dimension Lines). Based on the position of the mouse. Move the mouse. DL = [depending on the direction]) User defined (this option will require you to enter the prefix).15. 2.
plane of dimension line based on Z-axis plane of dimension line based on Y-axis plane of dimension line based on X-axis
The steps are the same as the steps of creating an orthogonal dimension line (see.2 Aligned Dimension Lines). Click on start point and on the end point of the first segment. 2. Click on start point and on the end point of the second segment. as the symbol of the angle between two segments. supplementary angle or complementary angle dimension can be entered.User’s Manual
47
Prefix
Sets the prefix used with the text on the dimension lines.9. In this case you have to select the direction X. the angle.
Aligned Dimension Lines Assigns aligned dimension lines or a string of dimension lines to the model. The position and radius of the angle dimension will be determined by the mouse movement.
Suffix
2.

To assign this symbol to an arc click any point of the arc and drag the symbol.15.
2.9.
Arc Length Creates arc length dimension symbols in your model.48
AxisVM 8+Release 4
By clicking the Units and formats button the angle number format can be set in the Dimensions section of the Settings / Units and Formats dialog box. To assign this symbol to a full circle click any point of the circle and drag the symbol.4. To assign this symbol to an arc click any point of the arc drag the symbol.
Arc Radius Creates arc radius dimension symbols in your model.9. click the middle point of the arc and drag the symbol.
. To assign this symbol to a part of an arc click any endpoint of the arc.5.15.
2.

By clicking the Units and formats button the number format can be set as the unit of Distance in the Geometry section of the Settings / Units and Formats dialog box. This is the unit and format used in the Coordinate Window.
Level Elevation
Selects the level mark symbol.15. Click on the point you want to mark. The top view is defined as the view in the direction of gravity (You can change it in the Settings / Gravitation dialog).
Sets the level and elevation mark parameters. by following the next steps: 1.7 Gravitation Elevation marks can be placed in front view. Selects the elevation mark symbol.9. Move the mouse in the direction you want to place the elevation mark. and sets its size and format.. and sets its size and format. side view. 3.User’s Manual
49
2.
Level and Elevation Marks Creates associative level and elevation marks in your model. See.3. by clicking on the desired point.. 2. and click to set the symbol in its final position.3. See.6.
. or in perspective.3.6 Units and Formats Level marks can be placed in top view...

2.9. You can reload and change default settings. Move the mouse to the desired position and click to set the text box in its final position. frame.
Text Box Creates an associative text box in your model. Click on the point to which you want to assign the text box. the transparency and alignment of the text. and the d distance of the extension line from the reference point (to which the text box is assigned to).50
AxisVM 8+Release 4
2. or in case of a single line text enter it directly into the edit field of the Toolbar.
You can create a text box in the following steps: 1.7. The text will use the same text formatting within a text box.
Color Text box
Sets the color of the text. style and size. Enter the text in the Text box parameters window. 3. Sets the text font. and extension line. You can enter multiline text in a text box. apply text box or font parameters to all existing text boxes
Font
. and extension line. You can get the color from the layer. These switches set the drawing parameters of the text box. frame.15.

doc If no full path is specified AxisVM starts from the folder of the model. For example an My result text box is displayed only when the My component is selected as the current result component. The steps of result labeling are similar to creating a text box.g. www.8. ftp://.. Information text box parameters can be set in a dialog:
Object info text box
Result labels
When displaying results the cursor determines the value of the current result component on nodes. A file reference is made of the -> characters and a file name. g. the first one is used.9. If the text contains a file reference or a link to a web page clicking the text box launches the application associated to the file or URL instead of opening the above dialog.
Object Info and Result Text Boxes Element or load properties appear in the text box depending on the current tab (Geometry. movies. So if our model is in C:\MyModel we can enter: -> \Reports\Details.. E.
. Element or Loads).. file://. sounds.. Clicking the text box the default web browser launches and opens the web site or file... surface centers.: ->C:\MyModel\Reports\Details. https://.. Excel tables or other documents to any part of the model. mid-side nodes.doc Clicking the text box starts the application associated to the file type. If the text contains more than one URL. The result text box is visible only when the selected result component is the same as the one that was selected when the result text box was created.
File reference
URL
2. To change the text select text box first (e... Shift+click) then click into the box.15... .User’s Manual
51
Active Links
Active links can be placed in text boxes to attach any external information tot the model. The text of the tooltip is automatically entered in a text box.. Supported protocols and link formats are: http://.. This way we can attach pictures. or intermediate points of beams or ribs and shows it as a tooltip..

For this result component only Result label is visible only if its result component is displayed. The actual values will be updated on changing the case. combination or description of the critical combination.
.
Result label text options : Element: Component: Case: Unit: Include element type and number. For all result components Result label remains visible regardless the displayed result component. Include unit name. In all load cases Result label remains visible regardless the load case. Include result component name. Include name of the load case.52
AxisVM 8+Release 4
Result text box options can be set in a dialog box:
In this load case only Result label is visible only in the load case in which it was created.

1. Apply parameters to all text box After clicking the OK button parameters of all text boxes will be set to these values. Click to the Isoline labels icon 2.9. Enter two points defining a line segment 3. This function is also available from the menu as Settings\Layer Manager.User’s Manual
53
Below the button of Use defaults three c heckboxes helps to customize the text box: Apply font to all text box After clicking the OK button only the font of all text boxes will change. See.15...3 Layer Manager
[F11]
2. The labels are placed at the intersections of the segment and the isolines
. Layer Manager Lets you create new layers or modify existing ones. 3.9. Save as default setting New text boxes will appear using the current settings as default.3.
Isoline labels Lets you place a series of labels to isolines.

10.and postprocessing easier. When the selection menu appears. you can enter in the Name field the name of the newly created part. This command will not affect the model.15. You must assign a name to each new part. (. Lets you modify the selected part. If more than one part is turned on n parts is displayed. ) characters in the name of a new part.
You can activate an existing part by clicking its name in the list box. called active parts. You have to specify the set operations.54
AxisVM 8+Release 4
2. double click on the respective name in the list. where n is the number of active parts. -. you need to put the name between “” marks (example: "floor +12. Lets you delete the definition of all the parts.00"). Working with parts makes the pre. Clicking on the Create button. Parts
Lets you create sets of structural elements called parts.
. at the same time. You must then define the new part by selecting entities (using the Selection Icon Bar if necessary) in the active display window. Lets you delete the selected part from the list. For example: %Columns will create the part that will include the entire model less the part named Column. In addition.
Modify Delete Delete All Logical Set Operations
If you want to use the +. the entities of the model that are in the part are displayed as selected. The name of the current part is displayed in the Info window. AxisVM allows you to display one or more parts. Parts can also be activated without opening this dialog box by simply clicking the Parts speed button (at the bottom of the screen). Creates a new part by performing logical set operations on the parts of a model. Use the % symbol to include the entire model. . New Creates a new part (a set of model entities). if the Parts check box is enabled the commands will only affect or refer to the entities of the active parts. To enter the name of a part. No part of the model is deleted.

If a truss.
Auto Refresh If it is on turning on or off parts will immediately cause a redraw. etc). If it is off the entire model is displayed.15.
2. Refresh all If it is on parts will be turned or on off in all window panes in multiwindow mode. Show non-visible parts grayed If it is on the entire modell wireframe is also displayed in gray to help identification of model parts.11. that can be used to process the results (displacements. rib or beam is within an active section plane and the result component has values on these elements a diagram is displayed on these line elements too. If it is off part settings will be updated only in the active panel.
. Sections
Lets you create section lines and planes through any surface model. internal forces. Parts If it is on only the parts checked in the list are displayed.
F
When working on parts. If it is off the screen is updated only after clicking the OK button. only the data of the active parts will appear in the tables by default.User’s Manual
55
Display switches
Display switches work in the following way: All Turns on or off all the parts in the list.

New section segment To define the segment enter two points of a domain or on domains in the same plane. Section lines. Setting the radio buttons you can control how the internal forces diagram will be displayed. planes and segments. If the result display mode is Section result diagrams are displayed only on section lines.
. Click or enter two points to set the section plane. This type of section is based on a plane.56
AxisVM 8+Release 4
The dialog works similar to the Parts dialog. In the Display Parameters dialog this parameter can be turned on/off for all section segments. Section planes are useful when you want to display results only along a certain line through the entire structure. Section planes are displayed as rectangles of dotted lines. planes or segments can be controlled to appear only in a certain load case and/or for a certain result component. Then click OK in the Selection Icon Bar to save. Diagrams are usually displayed perpendicular to the element plane but checking the option Draw diagram in the plane of the elements rotates the diagram into the plane. Left or right segment width can also be specified. To reduce the complexity of drawings display of individual sections lines.
Display of the resultant integrated values
Display of the average values New section plane Click New section plane and assign a name to the section. In perspective view you have to click or enter three points to set the section plane. planes and segments can also be turned on and off using a speed button at the bottom toolbar. You can enable/disable the display of section plane rectangles.

User’s Manual
57
New section line
Click New section line and assign a name to the section.
2.
F
The tracelines of the section lines are not correlated with the directions of the result components displayed.12. New.13. and moves the cursor over it. Section lines can be discontinuous. planes and segments are active. The checked section lines. You then have to select surface edges or beam elements that define the section line.
2. Find
Finds the entity having a specified index. You can use Auto Refresh and Refresh All checkboxes. Then click OK in the Selection Icon Bar to save.15.15. Modify and Delete buttons the same way as in the Parts dialog. If Select element is turned on the element found will also be selected (displayed in purple). Display Options
.

Color codes: axial displacement=yellow.
. any setting change will result in an automatic refresh of the active graphics window display. Surface center Enables the display of the center point (selection point) of the surface elements. $ Nodal supports appear as thick axes. shell = green. Symbols Graphics Symbols Enables/disables the display of the symbols. crosshairs or triangle. Node Enables the display of the nodes (small black rectangles). Surface support Enables the display of the surface supports.58
AxisVM 8+Release 4
Auto Refresh: If enabled. $ Node-to-node link elements are displayed as solid green lines with an arrowhead showing the location of the link. $ An orange line along the member and the number of the member. $ When disabled only the outlines are displayed. membrane = blue. membrane = blue. Mesh Enables the display of the inner mesh lines. Domain Enables the display of the domain’s contour. $ Surface supports appear as a light brown hatch . Line-to-line link elements are displayed as solid green lines with an arrowhead showing the location of the link and dashed green lines at the line endpoints. Edge support Enables the display of the edge supports. Cross-section shape Enables the display of the shape of the cross-section of the truss/beam/rib elements. Nodal support Enables the display of the nodal supports. $ Color codes: plate = red. Reference Enables the display of the references. $ Edge supports appear as a thick edge. $ The color of the domain is the same as of the surface type. End release: hinge / roller $ Blue circle: Blue circle + cross semi-rigid hinge Red circle: spherical hinge Solid blue circle: plastic hinge Edge hinges: $ Circles on the edges. axial rotation= orange. Color codes: axial displacement=yellow. $ The user-defined cross-sections will be displayed as rectangles that circumscribe the shape of the cross-sections. Center of circle $ Enables the display of centers of circles as a small cross. $ Red vector. shell = green. Refresh All: If enabled. End releases Enables the display of the end release and edge hinges. the changes will affect the settings of all graphics windows. Links Enables the display of link elements. Structural members Enables the display of the structural elements. axial rotation= orange. Color codes: plate = red.

temperature. distributed along a line.
Beam element local coordinate system
Surface element local coordinate systems Loads Display of load symbols can be set separately for each load type (concentrated.
. Changes will affect all panels in multi-window mode. miscellaneous (length changing. To display the derived beam loads check Derived beam load.
Derived beam load Auto Refresh Refresh All
Displaying of derived beam loads If it is turned on any change in settings will make the active panel redrawn immediately. distributed on surface. Local Systems Enables the display of axes of the elements in the local coordinate system. tension / compression). Mass Enables the display of the symbol of the concentrated masses.User’s Manual
59
Reinforcement parameters Enables the display of the assignment of reinforcement parameters to surface elements. self weight. To display of surface loads distribution to beams (see the diagram on the right) check Load distribution. $ Double red circle.

. materials.60
AxisVM 8+Release 4
Labels
Numbering
Displaying the number of nodes. See. crosssections..17. Info Enables the display of the Info window.3 Color Legend Window
. Properties
For meshed line elements checking Use finite element numbers displays the number of finite elements instead.17.17. cross-sections. See. 2.2 Coordinate Window.. 2. the labels will include the units as well.. masses. See. 2.
Enables the display of the name and values of materials properties.1 Info Window Color Legend Enables the display of the Color Legend window.. load values. elements. If the Units option check-box is enabled.
Switches
Information Windows
Coordinates Enables the display of the Coordinate window. element lengths or thicknesses. references..

Grid and Cursor Grid The grid consists of a regular mesh of points or lines and helps you position the cursor to provide a visual reference.7. Y or Z) one step (∆X. When using with constraints. Options
Allows the selection of the options for the settings of the grid. Guidelines Enables/disables the display of the guidelines. lines in gray.
2. drawing parameters. Depending on its type the grid is displayed as: Dot grid – axes are displayed with yellow crosses .. In such a case. the cursor will move along the line.14.14. ∆Z Sets the spacing of the dots/lines of the grid in the direction X.
. the cursor step is applied in the constrained direction with the DX value. Type Sets the type of the grid. and design code. ∆Y. editing.1. points in gray Grid lines – axes are displayed in yellow. cursor. nodes will be placed snapped to the grid. ∆Z Restricts the cursor movement to regular intervals.15. Ctrl x Sets the value of a factor that increases or decreases the cursor step size if you press the [Ctrl] key when you move the cursor.User’s Manual
61
Display
The display of the actual parts and guidelines can be turned on and off. Parts Enables/disables the display of parts. 4.15. ∆Y. Cursor Step Allows to choose coordinates of an invisible dot mesh (not the grid). Y or Z. This allows you to achieve adequate positioning accuracy. You can set the cursor step parameters as follows: Mouse Grid Restricts the movement of the mouse cursor to an invisible grid specified by the cursor step values below.
You can set the grid parameters as follows: Display Displays the grid if the check-box is enabled. ∆X. See.
F
The cursor step is ignored if you position the cursor on a line. ∆X. Each time you press a cursor movement key the cursor moves in the corresponding direction (X.
2. ∆Y or ∆Z respectively)..4 Constrained Cursor Movements
F
If the grid step and the cursor step is set to the same value.

Plane tolerance can be specified in two ways: Relative [‰] Absolute [m] per thousand of the biggest extension of the element polygon a given value
Auxiliary coordinates
Cylindrical or spherical.. See. This value is also used when comparing surface thickness or beam length. 4.4. Part management : Any entity drawn or modified after the check-box is enabled will be associated with all of the active parts. If two nodes are closer than the value set as the editing tolerance. Editing Constraint Angle During the model editing the movement of the cursor can be constrained. If more than one element is within this range the closest one will be identified.3.15.2 Polar Coordinates
. the movement direction can be set. Refresh : Sets the display refresh mode to automatic.. In this case the constrained movement of the cursor will be based on two types of angles (for other type of constrained movements see.. The unit for cursor identification distance is pixels.62
AxisVM 8+Release 4
2. they will be split. At intersection points of lines a node will be generated and lines will be bisected. they will be merged in the case of a mesh check.2.1 Cursor Identification
Editing Tolerance
Cursor identification
Plane tolerance
Nodes of domains and surfaces must be in plane.7. If surfaces are intersected by lines.7. See.14. Using the [Shift] key while moving the cursor.. and the resulting elements will have the same material and cross-sectional properties as the original.. If a node of a domain or surface deviates from this plane more than the given value the element will be deleted. Intersect : Sets the line intersection handling. 4.
n × ∆α custom α+90 ο custom α
Auto
Sets commands that are applied automatically if the corresponding check-box is enabled.4 Constrained Cursor Movements).. The element under the cursor is identified if it is within an adjustable cursor identification distance.

14.15.
Displayed edge Edge not displayed
Contour line angle
Zoom factor
Sets the scale of magnification/reduction of the zoom commands associated to the [+] and [-] keys. Sets the display of the inner mesh lines (between adjacent surface elements). The common edge of two or more surface elements is displayed if the angle enclosed by the normal to the planes of the elements is larger than the value set here.15. Line / surface load Sets the display size of the symbol of line / surface loads. Drawing Load symbol display factors Sets the display size of the load symbols. Force Sets the display size of the symbol of concentrated force loads. These values do not affect load values.3.User’s Manual
63
2.15.
. This factor is applied when the checkbox in the Symbols icon / Graphics Symbols / Load is enabled. Model Info
Shows the main parameters of the model. Moment Sets the display size of the symbol of concentrated moment loads.
2.

Coordinate Window
See.17. Information Windows
The information windows are situated in the graphics area. Info Window
Shows information about the display of the results such as: active part(s). E(EQ) parameters see Analysis and Static Analysis. current design code.
2. type of analysis.16. current load case or load combination. current perspective setting.17. Speed Buttons
The quick switches toolbar allows you to change the display settings without entering the Display Option/Symbols or Options dialog.4 Coordinate Window
. For the explanation of E(U). The icons are located in the bottom right corner of the graphics area. E(P). solution errors.64
AxisVM 8+Release 4
2. 4.17.. E(W). holding down the left mouse button..
Auto Intersection Mouse Snap Parts Display Parts of the selected elements Workplanes Section Lines & Planes & Segment Display Mesh Display Loads Symbols Display Symbols Display Local Systems Numbering Background Layer Background Layer Detection
F
Some of these settings are available also from Display and Service icons.1.
2. You can move these windows on the screen by clicking title bar.
2. current result component. and dragging it to a new location on the screen.2.

Color Legend setup
Limits
Setting criteria for the interval limits: Min/max of model Sets the lower and upper limit values to the minimum and maximum values of the entire model. If you enter a new top or bottom value the recalculated series will be linear between top and bottom values. The intermediate values are interpolated. To open this dialog box simply click the color legend window. By step value Color values are determined by the given step ∆. When entering a new level value the other levels will be recalculated using the step. Min/max of parts Sets the lower and upper limit values to the minimum and maximum values of the active parts. Intermediate values are interpolated.17. You can resize the window and change the number of levels simply by dragging the handle beside the level number edit box or entering a new value. Abs. The intermediate values are interpolated. max of model Sets the lower and upper limit values to the maximum• bsolute value of a the entire model with the respective negative and positive signs. You can set the color legend details in the color legend setup dialog box.e. linear between the top and the new value and between the new and the bottom value but steps may differ.User’s Manual
65
2.
. If you enter a new value at a middle interval the recalculated series will be bilinear. If you are in editing mode you can navigate through the list by UP and DOWN keys and edit the current item. Color Legend Window
Displays the color legend corresponding to the result component being displayed in the postprocessor. Switching from other crieria the array starts from the lowest value and using the latest step value. Custom Click an item of the list on the left to edit its value.3. Colors will be updated immediately. i. Intermediate values are interpolated. Auto Interpolate If Auto Interpolate is checked the series will be recalculated each time you enter a new value. Abs. max of parts Sets the lower and upper limit values to the maximum• bsolute value of a the active parts with the respective positive and negative signs. When you click OK the series of interval values must be monotonically decreasing from top to bottom.

.. To activate popup menu click right mouse button on the window.
F
When displaying actual reinforcement schemes AxisVM does not assign color to numerical values but to different rebar configurations. button.4.
2. Standard interval limit settings are also available directly from the color legend window popup menu. 2.17.. It can be set to display all schemes or just those within the active (visible) parts. Calculate When displaying reinforcement values click Custom and Calculate to get the amount of reinforcement from rebar diameters and distances for the selected list item..66
AxisVM 8+Release 4
You can save the settings of the scale using the Save As button.3 Views
. Perspective Window Tool
See. To review saved settings click the .15.

The Main Menu
3. You can enter specific information in the Heading section.
New Model
Creates a new untitled model.
. that will appear on each printed page. Use this command to start a new modeling session.1.1. If you have not saved the current model. Refer to the Save and Save As commands for more information on how to save your current model. You must specify a name for the new model. a prompt appears asking if you want to save it first.1. File
The menu commands are described below.
3. You can select the appropriate Standard and system of units.User’s Manual
67
3. A new model uses the default program settings.

AxisVM saves your model data in file names appearing as Modelname.
Open
[Ctrl]+ [O] Loads an existing model into AxisVM. Both file contains the same identifier unique for each save which makes it possible to check if AXS and AXE files belong to the same version of the model. a prompt appears asking if you want to save it first.2.
Converting models
Models created with previous AxisVM versions (if applicable) will be converted into the current version file format when you open them for the first time.AXS (input data).1. but want to keep the original version.
F
. If you enable Create Backup Copy check box in the Settings / Preferences / Data Integrity / Auto Save a backup file of your previous model will be created.68
AxisVM 8+Release 4
3. Selecting this menu command will bring up the Save As dialog box. but want to keep the original version. and Modelname.0 formats. Use the Save As command if you are changing an existing model. Selecting this command will bring up the Open dialog box. If the folder name appearing in the dialog box is what you want. If the directory is not what you want. select the drive and directory names along with the file name. the Save As dialog box automatically appears prompting you to enter a name. or if you are changing an existing model. Refer to the Save and Save As commands for more information on how to save your current model. The File / Save As / File Format command lets you save the model in Axis version 5.4. Use this menu command to name and save a model if you have not saved the model yet. If you have not saved the current model.
3.
F
Current drive
Model data files in the current folder
Model info
Model display
3. simply enter the file name in the edit box or select it from the list box.1.
Save As
Names and saves the model.0 / 7.0 / 6.
Save
[Ctrl]+ [S] Saves the model under the name displayed at the top of the AxisVM screen.AXE (the results).3. If you have not saved the model yet.1.

that lets you specify the units of measurement in the exported file.5. Creates a DXF file to use in CADWork reinforcement detailing software.stp) Saves the data of the truss and beam elements (endpoints. Revit. in a Modelname. The file includes the coordinates of i and j-end nodes. loads and the calculated results of the selected beam elements. Selecting this menu command will bring up the Export DXF dialog box.
Bocad file
StatikPlan file
PianoCA file IFC 2x. . AutoDesk ADT. Three different formats are available for DXF output. Z coordinate represents the calculated amount of reinforcement.1.5. beams). Exports only the elements that are in the current selection set. Exports an IFC file describing the model with achitectural objects (walls. The default unit is meter [m].apx file is present in its AddOns folder.AutoCAD reinforcement design file
AOF file
Frame structure models should be exported in AOF (AxisVM Object File) format to ArchiCAD 6. supports.User’s Manual
69
3. cross section. Nemetscheck Allplan.DXF file.asc) Saves the geometry of the model into a file format that is recognized by the Xsteel software. As CADWork works in 2D. 6. The geometry is saved with actual dimensions. slabs. Saves the geometry of the model into a file format that is recognized by the Bocad software. DSTV file (*. selected domains must be in the same plane. The file includes the coordinates of i and j-end nodes. Tekla-Xsteel and other architectural programs.0. For StatikPlan AxisVM exports a DXF file including the contour of the reinforced concrete plate.0.
Export
DXF file
Saves the geometry of the model to a DXF file format for use in other CAD programs. Generates a *. or 7. material. reference) as a standard DSTV file. the calculated reinforcements as isolines and the result legends on different layers. This file format is supported by several steel designer CAD software.AutoCAD R12 DXF file . Each domain in the DXF file is transformed to a local X-Y coordinate system. IFC files can be imported in ArchiCAD. the cross-sectional properties and the reference point of truss and beam elements.AutoCAD 2000 DXF file . the cross-sectional properties and the reference point of truss and beam elements.
F
Xsteel file
ArchiCAD can read the aof file only if the Axisvm. Two different file formats are available: XSteel ascii file (*.pia interface file for PianoCA. 2x2 file
CADWork file
Export Selected Only Coordinate units
. columns. Only selected domains will be exported. It includes the data. The coordinate units of the exported file can be selected here.

..1. the Layer Manager will ask if you want to update the layers.3. specifically for Graphisoft ArchiCAD software. To save an ArchiCAD model as ACH file you must follow within ArchiCAD the steps below: 1.18 Creating model framework from an architectural model
F
In order to be able to export an ACH file from an ArchiCAD project.9. Select the AxisVM file format option 6. Enable the display of the levels and objects that you want to be included in the analysis 3. If the file date of the imported file has changed. Apply the Save As command (File menu) 5. The layers of the imported file are loaded into the Layer Manager (see. 13. If you have an existing ArchiCAD model the new model always overwrites it.6. Close the Save As dialog with the OK button.apx file is copied from your AxisVM setup CD to the ArchiCAD 6. See.
F
Import Model
The ellipses will be converted to polygons only if you load them as active mesh otherwise they remain ellipses.. The ACH file format was developed by Inter-CAD Kft. AxisVM generates the cross-sections from the geometric data of the corresponding ArchiCAD objects.. Open the ArchiCAD model file 2.ach) and specify the folder where you want to save the file 7. 14 and 2000 format into AxisVM.dxf
Imports a geometry mesh from a DXF file (drawing interchange file) exported in AutoCAD 12. in order to allow integrated design of complex structures architecturally designed with ArchiCAD and numerically analyzed with AxisVM. Select a perspective display of the model 4.3.70
AxisVM 8+Release 4
3. Selecting this menu command will bring up the Import DXF dialog box.
.
AutoCAD *. Enter a filename (the file will be saved as filename. 4.0 (or later version) AddOns folder.3 Layer Manager).ach
Imports an object-oriented mesh from an ACH file into AxisVM. you have to make sure that the Axisvm.
Import
ArchiCAD *.

Import As You must specify whether you wish to use the imported DXF file as an active mesh or as a background layer. Imports objects from an architectural model saved as an IFC file. Import Mode Place You can choose between overwriting the former geometry or adding a new geometry to the former one Lets you specify the plane of the DXF layer (X-Y. You must always set this to a small number relative to your model dimensions. Background layer The imported geometry is used as a background layer that is displayed but is inactive as a mesh. The Place button allows to graphically position the imported DXF drawing in your model space.9. The coordinates of the merged points (nodes) are averaged. You can use the entities in the background layer as a reference during editing your model. 2x3 *. to them. Revit Structure.
Geometry check tolerance When you import a DXF file as an active mesh. 2x and 2x2.
.User’s Manual
71
Parameters
Input units You need to specify the length unit used in the imported DXF file... Maximum deviation from the arc [m]: Importing a DXF file as an active mesh. and merges them. ellipses will be converted to polygons based on this value. Revit Building Nemetscheck Allplan.18 Creating model framework from an architectural model
IFC 2. AutoDesk Architectural Desktop. You can specify the maximum distance to merge points. If the AxisVM model already contains an architectural model it can be overwritten or updated in the import process. Imported objects can be displayed as a 3D background layer or can be converted to a native model by assigning materials. You can import object based architectural models from ArchiCAD. Import a DXF file as background layer when you want to create the model based on architectural plans or sections. Points that are closer together than the specified distance are considered to be coinciding. 4. Existing architectural models are always overwritten by the new one. or Y-Z). Active mesh (nodes&lines) The imported geometry is considered as if it were created with AxisVM commands.0. See. cross-sections etc. X-Z. Programs. Bocad and Xsteel.ifc file
F
When exporting a model from ADT (Architectural Desktop) turn off the automatic intersection of walls before creating the IFC file. AxisVM checks for coinciding points (nodes) and lines in your model.

Opens a data file created by Bocad steel construction software (*. If no load groups or combinations are defined in the imported model. and merges it with the current model.BAT !REGISTER_TEKLA. the load in the current model will be retained. Multiple nodes and degeneated triangles are filtered out..g.sc1 file Reads the triangular mesh describing the surface of a model from a file in STL format. otherwise they are appended. When importing an AxisVM file the following dialog is displayed:
Use the Place button to graphically position the imported model in your model’s space.8. the properties of the current model will be retained. in the Analysis menu then click the Properties button to set AxisVM AD Engine as the Analysis engine. Section 4.. To make the connection work first the COM server must be registered within the operating system (in the Registry) then Tekla Structures must be notified that a compatible server is available.
3.1.11) command is automatically applied..axs
Imports a model from an existing AxisVM file into AxisVM. Stereo Lithography *.sc1) and imports beam cross-sections and geometry. Setup
Tekla Structure – AxisVM connection The connection between the two software is made through a COM server enabled to run AxisVM. the loads will be merged. The Section Lines/Planes Parts with the same name are merged. If the same case exists in both models.BAT
If connections fails any time it is recommended to run this registration again. Load groups and combinations if any. Connection After a successful registration the model built in Tekla Structures can be transferred to AxisVM in the following way: click Analysis & Design models.. the Geometry Check (See.
. however if Tekla Structures is not installed the second registration cannot be completed.stl file Bocad interface *. If both models contains loads that are limited to one occurrence (e. AxisVM setup automatically performs these registering operations.72
AxisVM 8+Release 4
AxisVM *. thermal) in the same load case. During the merging process. the load cases will be appended to the existing ones as new cases. are appended to the existing ones as new groups and combinations.6.1. Therefore after installing Tekla Structures the registration has to be started again by running two batch files from the AxisVM program folder
!REGISTER_AXISVM. If there are different properties assigned to the same merged elements. and the load cases as new cases.

User’s Manual
73
If AxisVM AD Engine does not appear in the dropdown list the registration was not successful and has to be repeated. Getting back to the Analysis & Design models dialog click Run to start the transfer of the model.
. The process status is displayed in dialog. If the transfer is completed successfully click the OK button to see the model in AxisVM.

It will appear on the top of every printed page.
.74
AxisVM 8+Release 4
The model transferred to AxisVM:
Loads and load cases specified in Tekla Structures are also converted.
3. which contains the name of the project and designer.
Page Header
Lets you specify a header text (two lines).7.1.

and of the page.
Output Current printer Printer setup
Printing drawing
Send To Lets you send the output directly to the printer/plotter or to a graphics file (DXF. mm or cm and bitmap resolution in dpi (dots per inch).User’s Manual
75
3. BMP or Windows Metafile [WMF/EMF]).
3. Margins (Printer/DXF) Lets you set the size and the units of the page margins. You can also drag margin lines within the preview area by their corner and midside handles. By pressing the left mouse button and moving the mouse you can specify an additional panning which will affect the printed output only. You can set the number of copies required. The Setup button invokes the standard Windows Printer Setup dialog where you can change printer and printer settings in detail.1. If you select Printer as a target the graphics cursor turns to a hand whenever it enters the preview area. Preview Lets you view the printed image prior printing. This is a standard Windows dialog therefore its language corresponds with the language of the installed operating system. If a file is selected as output.9. Scale Lets you set the scale of the drawing to print.
Print Setup
Allows setting the parameters of the default printer.
Print
[Ctrl]+ [P] Lets you print the model according to the current display settings. where Name is a file name to be entered.
. In case of perspective or rendered view or if the output is sent to a Windows Metafile the scale cannot be set.prn file.8. Printer Lets you select and setup the printer. Allows the setup of the printer. JPG) Lets you set the bitmap size in pixels. the printing will be stored in the Name.1. inch. Bitmap Size (BMP.

When black and white printing is selected.
. Thick lines are used for drawing supports and rigid elements. Change Fonts Lets you select fonts to be used in printing and set the font size. If your printer cannot print in color you may get different results in the first two cases. Thin lines are used for elements and geometry and other entities.prn already exists. Paper size Lets you set the size of the paper. If you want to print only into files. Medium lines are used for isolines and section line. you can set the operating system to do so in the Start/Settings/Printers choosing Properties and setting the Print to the Port as File. Try both to find which works better for you. and the starting number for the page numbering. all entities are printed in black. If you select Colors the conversion to grayscale will be performed by the Windows printer driver. Pen widths Sets the size of the pens for printing. name. Orientation Lets you set the orientation of the page.
Windows to Print Lets you print either the active window or all windows displayed. or black and white. Printing to file When Print to File is selected the printing is redirected to a file. If you select Grayscale the output will be converted to grayscale using an internal grayscale palette of AxisVM. or overwrite it. color.76
AxisVM 8+Release 4
Page Header Lets you set the date and remark that will appear on each page. In this case you can not append print files. If the file name.prn that you can print anytime later. you can add your printing to it. Color Options Lets you select printing in grayscale.

3.
.1. 20-18 in the Selected field the 1 st.
You can print more than one prn file at a time. 9 th. 7 th. 3.10. you can set the pages (all/even/odd) of all/current/selected pages you want to print. and 18th page will be printed in this order. You can set the printing order with the up/down arrows in the right of the file list box. Printing from File
You can print the prn file you created from the following window. or dragging the file names to a new position with the mouse. 10th. 19th. 3 rd. Example: Entering 1. 20 th. 8 th. 7-10.User’s Manual
77
Printing table
When printing from the table browser.

78
AxisVM 8+Release 4
3.
.11.
$
The AxisVM model files are marked with the symbol. get information and manage your model files. the bottom right
Preview Shows the model wireframe in front.
Current drive Current folder
Current model preview
New Creates a new sub-folder in the current folder with the name you enter. Copy Copies the selected files to a different folder. You can specify to delete only the result files or all. . Model Library
The File/Model Library command lets you preview. Model information is also displayed in a list. but in the list box you can select multiple files.1. As in Open and Save As dialog windows the standard file access dialog box items are displayed. Open Opens the selected file for editing. top view or in perspective depending on the model dimensions. If a model has a result file the symbol has a blue right-bottom corner.
.
$
AxisVM files are marked with corner of the icon is blue. If a result file is available. Rename/Move Renames the selected files in the current folders or moves them into a different folder. Delete Deletes the selected files from the current folders. side. You can specify whether to copy the result files or not. Close Quits the Model Library.

or delete existing material data..9. In case of entering a new material with an existing name it will be added as materialname_number. national design code. Material Library
AxisVM provides a preloaded material library (that contains the most frequently used structural materials) and allows you to create material property sets that you can use over and over again in many different models. DIN-1045. Properties of materials This table contains the properties of materials often used in civil engineering to the MSz. (see. Eurocode.
F
Changes in the material library does not reflect in models using the modified material. the following dialog is displayed: Definig new material or clicking to a non-editable column (eg. a STAS and Italian codes. You can add.6 Line Elements. 4. in which all material properties.12. modify.9.. SIA-162. When a material with a name identical to one existing is entered an index is attached to the name (name_index) to differentiate from the existing one. NEN. When entering a new material. See the detailed description of the Table Browser in section 2. 4. DIN-1045-1.18 Creating model framework from an architectural model).9.User’s Manual
79
3. type) a dialog appears. calculation and design parameters can be defined or changed.
The material library window can also be opened using the Table Browser icon and by selecting Libraries/Material Library.
Define new material [Ctrl+Ins]. You must assign different names to each material property set. The fields containing the basic properties independent of the design code can be edited in the table. These materials can be used in any model.1. Change material properties
.

and specify the following properties: Name Fabrication process Shape Rolled. Z.1. Custom
Cross-section properties
When creating a new cross-section in the table all property values have to be entered.t(*) W2.pl(*) W2. bottom = I1 / e2_min Elastic cross-section modulus.p.zs S. T. cold-formed. other. I (H. library file name and a cross-section type. welded. el. top = I1 / e2_max (see diagram below) Elastic cross-section modulus. You have to specify library name. Box. and allow you to create standard cross-section property sets that you can use over and over again in many different models. S. W).b (*) W2. C. r 3 Ix Iy Iz Iyz I1(*) I2(*) Iω W1.User’s Manual
81
3. r 2. L. Cross-Section Library
AxisVM provides preloaded cross-section libraries. (*)
. that contain the most frequently used steel shapes and concrete cross-sections. el.t(*) W1.sec) are stored in the folder where the application is stored. J. Round. The libraries includes products of manufacturers worldwide.el.el.13. For the description of the Table Browser see 2. Standard and custom cross-section library files (*.pl(*) i1(*) i2(*) b h yG Axial (cross-sectional) area Shear area associated with shear forces in local 1st direction Shear area associated with shear forces in local 2nd direction Rounding (corner and fillet) radii Torsional inertia Flexural inertia about local y axis Flexural inertia about local z axis Centrifugal inertia Principal inertia about local 1st axis Principal inertia about local 2nd axis Warping modulus (used for the design of steel shapes) Elastic cross-section modulus.
F
Create a new library
The Undo function does not work when libraries are modified. Pipe. Ax A1(*) A2(*) r1. U. Rectangle. Assign a name to each cross-section. bottom = I2 / e1_min Plastic cross-section modulus Plastic cross-section modulus Radius of inertia about local 1st axis Radius of inertia about local 2nd axis Dimension in the local y direction (width) Dimension in the local z direction (height) Position of the center of gravity of the cross-section in local y direction relative to the lower-left corner of the circumscribed rectangle Position of the center of gravity of the cross-section in local z direction relative to the lower-left corner of the circumscribed rectangle Position of the shear center in local y and z directions relative to the center of gravity Stress calculation points If first and second principal axes are the local y and z axes values with (*) appears with indices y and z. You can create a custom cross-section library by the File / New Cross-Section Table command in the Table Browser.9 Table Browser. top = I2 / e1_max Elastic cross-section modulus.b(*) W1.
zG
ys.

The properties that were not published by the manufacturers were calculated. Custom library properties can be deleted by the File / Delete Cross-Section Table command in the Table Browser.13. You can add a new cross-section to any custom or standard library by Edit / New Row (or by pressing [CTRL+INS] or the toolbar button) in the Table Browser and entering field values.1.
Import/Export values Copy/Paste a crosssection
Add/Modify / Delete a crosssection
F
The table below shows the shape and reference coordinate system of the crosssections. You can delete a cross-section with the aid of deletion icon or by pressing [CTRL+Del]. You must verify them before use. You can also call the Cross Section Editor to specify cross-section data.
. The property values in standard libraries are taken from manufacturers’ databases. You can copy and paste cross-sections with their full graphical description within the Table Browser.82
AxisVM 8+Release 4
Table properties
Custom library properties can be modified by the File / Cross-Section Table Properties command in the Table Browser. See description of the cross-section editor in section 3. Numerical data exchange with other applications is supported via clipboard. Changing any dimension of a standard shape AxisVM automatically recalculates all cross-section parameters and updates the graphics. Cross-section libraries contain the values of the warping inertia Iω used in the Steel Design module. You can import and export numerical values in libraries as dBaseIII files by File / Import dBase file. Use Edit / Design New Cross-Section (or [CTRL+G]) to add a new cross-section and Edit / Modify Cross-Section (or [CTRL+M]) to modify an existing one.1.

copy or move the selected components at any time during the editing. rectangular.....8 Saving drawings and design result tables Undoes the last operation. rotate. Prints the cross-section. and saves your current cross-section into the cross-section table of your model with a name you specify.. mirror.
F
Icon bar
.1. 2. 4.9.
Cross-Section Editor The Cross-section Editor allows you to edit thin and thick walled cross-sections.
From Cross-section Library From DXF file
Loads a cross-section from the Cross-section Library. the Mouse Most important functions are available from the toolbar. Redo the operation which was undone. You can translate. Stress calculations are performed at the specified stress-points only. ring and polygonal shapes. The behaviour of the Icon bar is the same as that of the main Icon bar. 4.9. When a component is placed to its location graphically. You can use parametric circular. 2.18 Creating model framework from an architectural model
Editor Keys Toolbar
See. The only difference is that this Icon bar can be moved above the menus at the top or at the bottom but it is not dockable. Copies the image of the cross-section to the Clipboard.1. Editor functions and settings can be found on the Icon bar on the left. If you don’t specify any stress-points..1. the principal axes and the cross-sectional properties of the composite cross-section are computed. You can specify up to 8 stress-points for each cross-section. and have to be of the same material. the Keyboard.5 Using the Cursor. The default stresspoint is the center of gravity.2. or any shape listed in the cross-section libraries to edit composite cross-sections. Only thick or thin-walled cross-sections are available depending on the cross-section editor tab position. stress will be calculated in the center of gravity only. See.User’s Manual
85
3.6 Line Elements The editor can be used when creating a native model from an architectural model through the IFC interface.. Contour of thick walled cross-sections can also be imported from a DXF file. It means that no bending stress will appear. See… 3..15 Icon bar.. When applying a move command the stress-points can also be moved. The shapes used to build a new cross-section are referred to as components. See. 3. See..13. Cross-section editor is on the toolbar of the Cross-section Library and can also be launched from the line element dialog. See.9 Print Adds the image of the cross-section to the Gallery. The OK button exits and closes the cross-section editor window.
Stress-points
You can specify the points you want to calculate stresses for. You can use keyboard commands the same way as in main editing windows.

86
AxisVM 8+Release 4
Thin-walled crosssections
A component belonging to the thin-walled category can be added to your cross-section. welded. corner/fillet radius. Standard shapes can also be defined parametrically. web and flange thicknesses and a fillet radius.). Base-point You can select a base-point to each cross-section component.) Values depending on the type of the cross-section (height. The default value is 0. depending on its shape and final location within the composite cross-section. that allows you to position the component during editing. thickness. width.
Manufacturing process Dimensions Rotation I shape . cold formed. diameter etc. In this case the following parameters has to be defined in the dialog: There are three options (rolled. width. Lets you define a rotation by angle α. Wedged I shape
Definition of an I or wedged I shape by its height.
.

. width.
Before the definition the position of the control line of the segment can be selected: 1. web and upper / lower flange dimensions. width. Polygonal . which is displayed with a dashed line. Rectangular
Definition of a rectangle by its parameters b (width). thickness and in the case of rolled or bended cross-sections by the corner/fillet radius.
Other shapes . v (thickness). right side R parameter : Rounding (corner and fillet) radii
. Definition of cross-sections by height.
Definition of a polygonal shape.User’s Manual
87
Asymmetric I shape
Definition of an asymmetric I shape by its height. left side 2. Pipe Definition of a pipe by its parameters d (outside diameter). and v (thickness). The centerline is considered as the contour of a closed domain. . center line 3. and α. with b>v.

and closed polygonal. a3. L shapes. cursor step. I shape
Definition of a circular or semicircular shape by its diameter and α. circular. If the Contour button is down the cross-section can be defined.
Contour
Hole
. and closed polygonal shape components. Definition of an I shape by its parameters a1. circular. (b1. U. and select the components you want to delete.88
AxisVM 8+Release 4
Arc shape
Definition of an arc shape by its diameter. and α. b2. a3). central angle and thickness. If the Hole button is down a hole can be specified.
Polygonal
Insert a vertex
Insertion of a new vertex on the contour of the cross-section. h (height). Semicircular . When deleting a component the stress-points will also be delete. Delete Using the [Del] key you can invoke the Selection Icon Bar. Parameters can be set to 0. Stress-point Deletes the selected stress-points. You can specify a hole in rectangular. a2.
F
Options Thick-walled cross-sections
Rectangular
Definition of a rectangle by its parameters b (width). The hole can be rectangular. Lets you set the grid size. (a1. b3). Shape of the cross-section can be changed by dragging a vertex by the mouse. b3. You cannot delete the default stress-point (the center of gravity). b1.
Circular. and the zoom factors. and α. Definition of a polygonal shape by drawing a polygon. allowing the creation of T.

cursor step. Iz.t(*) W2.t (*) W1. ρ1. ρyz. z s Po Pi (*)
. ρy. top = I2 / e1_max Elastic cross-section modulus. and select the components you want to delete. Iyz by integration. ρz. el. Iω. and the zoom factors. You can not delete the default stress-point (from the center of gravity). top = I1 / e2_max (see diagram below) Elastic cross-section modulus.User’s Manual Delete
89
Using the [Del] key you can invoke the selection window.b (*) W2.
zG
y s. A 1. A2 by performing a finite element analysis of the cross-section. Iy. bottom = I2 / e1_min Plastic cross-section modulus Plastic cross-section modulus Radius of inertia about local 1st axis Radius of inertia about local 2nd axis Position of the center of gravity of the cross-section in local y direction relative to the lower-left corner of the circumscribed rectangle Position of the center of gravity of the cross-section in local z direction relative to the lower-left corner of the circumscribed rectangle Position of the shear center in local y and z directions relative to the center of gravity Outer circumference (cross-section contour) Inner circumference (holes) If first and second principal axes are the local y and z axes values with (*) appears with indices y and z. ρ2. the stress-points will also be deleted. Ax Ay Az Ix Iy Iz Iyz I1(*) I2(*) • Iω ρy ρz ρyz ρ1 ρ2 A1(*) A2(*) W1.el.pl(*) W2. Ix.el. A1. Az. ρz. Following cross-section properties are calculated:
F
Options
Compute properties
AxisVM calculates Ax. Ay.
F
In case of a cross-section consisting of two or more independent parts. Deletes the selected stress-points. When deleting a component. Warping modulus (used for the design of steel shapes) shear factor in local y direction shear factor in local y direction shear factor for local yz cross shear factor for local 1st direction shear factor for local 2nd direction Shear area associated with shear forces in local 1st direction Shear area associated with shear forces in local 2nd direction Elastic cross-section modulus. Az. ρy. el. ρ1.b(*) W1. ρ2. bottom = I1 / e2_min Elastic cross-section modulus. Lets you set the grid size.pl(*) i1 i2 yG Axial (cross-sectional) area Shear area in local y direction Shear area in local z direction Torsional inertia Flexural inertia about local y axis Flexural inertia about local z axis Centrifugal inertia Principal inertia about local 1st axis Principal inertia about local 2nd axis Angle between local 1 st axis and the local y axis. Polygon Stress-point Deletes the selected components. Ay. ρyz. A 2 are not determinded.

1 Selection. Enable the check-boxes of the entities you want to delete. In the dialog window the check-boxes are active or inactive according to the contents of the current selection set (intended for deletion).
Redo
[Shift]+[Ctrl]+[Z]
Undoes the undo command or goes forward to reverse one or more undo commands. To delete: 1.. Press the [Del] key.. 2. click the down arrow next to the Undo icon.
Delete
[Del] Deletes the selected entities.2..2. Lets you delete the selected geometric entities.15. See.
3. You can select the entities by holding the [Shift] key pressed while you click on the entities with the left mouse button or use the Selection Icon Bar.
3.1 Selection [Ctrl]+ [A]
3. If no elements are selected it brings up the Selection icon bar and then the Delete dialog window. Select the geometric entities to be deleted.2. If there is no selection.4. To undo a sequence of actions (more levels).2.User’s Manual
91
3.
•
Copy
Copies the drawing of the current graphics window to the clipboard.2. to finish and close the dialog window.
•
Select All
See.
Undo
[Ctrl]+[Z]
Undoes the effect of the previous commands. Press the OK button. You can select the actions you want to redo based on the time or type of the commands. 4. the selection toolbar appears and objects can be selected for deletion. and then select the actions you want to undo based on the time or type of the commands. 3.5.. 2.15. 2.
.1.3. [Ctrl]+ [C]
3. You can set the number of undo/redo levels (maximum 99) in the Main menu/Settings dialog box.2.

for deletion. text boxes etc. Lets you select the dimension lines.2. Lets you remove mesh from domains. 2. In case of a divided view you can select to save all windows or the active one only. but will delete the loads. bolted joint diagrams.2.. Drawings Library is another way to store diagrams. 2..
Report Maker
See.. nonlinear calculation results.. While Gallery contains static image files.10 Report Maker [F10]
3. Deleting geometric entities that have assigned finite elements.8.92
AxisVM 8+Release 4
Geometry
Elements References Mesh R.C. All finite elements that use the deleted references. will result in the deletion of its finite elements and of the associated loads. Deleting finite elements will not delete the respective geometric entity. beam displacement and internal forces diagrams.7.
3.. 2.9 Table Browser
3.13 Drawings Library
Add drawing to Gallery [F9]
F
. Lets you select the reinforcement parameters attached to the selected elements for deletion. Design Steel design Dimensions
Lets you select geometric entities for deletion.. steel design results. Lets you select the steel design parameters attached to the selected elements for deletion. Lets you select finite elements for deletion. and the associated loads will be deleted too. See. reinforced concrete column and beam design diagrams. the Drawings Library uses associative drawings following changes in the model.2.
Table Browser
[F12] See.
Saving drawings and design result tables
You can save drawings from AxisVM in many different contexts: you can save AxisVM main windows.6. Lets you select references for deletion.

3.EMF) store a series of drawing commands so they can be scaled and printed in any size in the same quality. However if you choose hidden line removal or a rendered view drawn by OpenGL technology metafiles will contain only bitmaps.WMF. Do not modify the name of the subfolder Images_modelname.10. . different material.11. per cross-section or surface type. JPG is a compressed format with a slight loss of quality but these files are much smaller than BMPs. Find structural members
AxisVM handles line elements as structural members. .9. A breaking point is defined by different local x or z directions. so Windows metafiles provide higher resolution when printed.User’s Manual
93
Which file format to use?
Bitmap formats (.
Weight Report
[F8] The weight of the entire model.3. To get a high resolution rendered view print the picture directly. cross-section or eccentricity.BMP. It means that Meshing of line elements on the Mesh tab creates finite elements but the line elements themselves are not divided.
3. Break apart structural members
The Break apart structural members menu command breaks apart line elements created with the Find structural members command. Settings
. These pictures can be inserted into a report. The Find structural members menu command joins adjacent line elements into a single element until a breaking point is found. end release or a domain boundary.2.
3. Line elements must be on the same line or on the same arc. selected elements or details can be listed in tabular form per material. Drawings will be saved to a subfolder Images_modelname automatically created under the folder of the model file.
3. Windows metafiles (.2.JPG) store the pixels of the diagram.2.

94
AxisVM 8+Release 4
3. 2.15. you can modify its properties in the right side (Name.3. 2.15. you can modify all the DXF layers at a time.. 2.15.... Display Options See. 2. Properties of AxisVM structural layers cannot be modified. If no AxisVM layers are defined AxisVM automatically creates a new layer for dimension lines with the name Dimensions.13.13..
.1.3. Color. Display Options
3. Options
3.
Layer Manager
[F11]
The Layer Manager allows you to manage AxisVM layers. If you select the main DXF file entry of the tree.15.2.3.14.
Display
Symbols [Ctrl]+ [Y] Labels [Ctrl]+ [L] Switches [Ctrl]+ [D]
See. Display Options See. imported DXF or ArchiCAD layers.13..
Options
See. Style.3. Size).. multiple DXF layers are allowed. If you select (highlight) a DXF layer in the tree. On the left side of the Layer Manager dialog a tree view of the available layers is displayed.. While only one ArchiCAD layer can be imported.

.
3.
Units and Formats
Lets you configure the units (SI and/or Imperial) and formats of variables used throughout the program (number of decimals used for displaying or exponential format).. or create and save your own custom sets.User’s Manual
95
Apply to All: When using this button.4.17. The visibility of the layers or DXF files can also be set by clicking on the bulb or cursor symbol next to the layer or file name. Deletes all imported DXF layer that are empty (contain no entities). 2. Changing Design Code changes the method of calculating critical load combinations therefore all load group parameters but safety factors will be deleted. Seismic analysis parameters and seismic load cases will also be deleted. line style and size. New AxisVM Layer Delete Delete Empty AxisVM Layer Delete Empty DXF Layer Creates a new AxisVM layer.3. More than one layer or group can be selected and deleted by the [Del] key.
Guidelines
[CTRL]+[G] Guidelines See.3.3.
Design Codes
Sets the Design Code to be used in case of code specific tasks.5.6. As material properties and certain reinforcement parameters are not the same in different codes it is recommended to revise the values you have specified. Deletes all AxisVM layers that are empty (contain no entities).15.
3. a dialogue window will allow you to select the items in the DXF layers that will have their properties set based on the layer’s settings. You can set the layer’s name.. You can use predefined sets as the SI set. color. Guidelines
3.

Preferences
Data Integrity
Recent file list
Lets you set the number of recently opened AxisVM model files listed in the bottom of the File menu.3.
Gravitation
Lets you set the gravitational acceleration constant and the direction of gravitation as one of the global coordinate directions
3. and set if you want the last edited file to be opened at startup.96
AxisVM 8+Release 4
3..2 Installation) will be shown on startup if the show welcome screen on startup checkbox is checked. The welcome screen (See.
. 2.3.8.7..

~AX. light gray or white). Disconnecting may also happen in a situation when you get a phone call and you do not use the program for a time longer than the network time-out. You have to specify the maximum number of actions you want to undo. numbers. In the Minutes box.
Colors
Lets you select graphics area background color (black.avm.User’s Manual
97
Save
Auto Save option To make sure that you do not lose your work. symbols and elements will automatically change their colors to remain visible. enter the interval at which you want to automatically save the opened model (1-99 minutes). Save derivative results If this checkbox is checked stresses.
Undo GroupUndo Network time-out
You can undo your last actions. Name of the backup file is modelname. Create Backup Copy If this checkbox is checked and a model is saved after making changes a backup copy is automatically created from the previous state of the axs file. This number must be between 1 and 99. dark gray.
. When you have to restart AxisVM after a power failure or due to any other problem that occurred before you saved your work. A model that is saved automatically is stored in the default temporary folder of the operating system (by default it is c: \ Documents and Settings \ username \ Local Settings \ Temp) as ~modelname. the current AxisVM session is closed. In case off network hardware protection keys. Labels.avm until you perform a save command. envelopes. AxisVM can recover it from the temporary file stored in the above folder under the name $modelname. The Group Undo option allows you to undo the effects of complex commands in a single step. If another user asks for access to the key the server gives a license to him/her and when you try to continue your work the program displays an error message and halts at the next key check. select the Auto Save option by the check box. You must still save the model when you exit. critical combinations and design results will be saved as well. if in a time period set here there is no activity (checks) with the key.

When launching the analysis missing meshes will be recreated based on the meshing parameters of the domain.98
AxisVM 8+Release 4
Fonts
Lets you change the typeface and size of the fonts that are used when displaying your model and the Floating Palettes. Remove and create mesh automatically Any editing performed on a domain deletes its mesh.
Mesh management
One of the following mesh management methods can be chosen. Its shows the distance of the cursor from the current workplane. Circle Closing Angle Projection line to workplane Meshing Parameter for drawing arcs. Keep mesh editable Meshes can be edited manually.
. If the center angle of the arc is smaller than this angle or it is closer to 360° than this angle then a whole circle will be drawn. Edit
Two general editing parameters can be set on this panel. Default settings can be restored by pressing the button on the right. Click white sample area to get to the font selection dialog. Display of projection lines can be turned on/off.

User’s Manual
99
Contour division method
Uniform mesh size Meshes will be generated according to the user defined element size regardless of the shape of the domain (least number of finite elements). Arcs are displayed as polygons. Clicking the arrow in the right bottom another toolbar flies out showing different tools. This parameter affects drawing only and is not related to the precision of the analysis.
Default mesh size Toolbar
Displaying toolbar
If Horizontal toolbars expanded is chosen. Separator lines indicate different groups of functions. The finer the resolution the closer the polygon will get to the arc. Pet palette position can be: Relative Specify the horizontal (dx) and vertical (dy) distance from the operation in pixels. When defining meshing parameters for a domain for the first time this value will appear by default. Set the display resolution here. Appear in the latest position Pet palette appears in its latest position. different functional groups will be represented by a single icon. Adaptive mesh size Takes the shape of the domain into consideration and creates a better mesh by increasing mesh density wherever it is necessary. all icon appears in a row.
. If Flyout toolbars is chosen.
Pet palette position
Display
Moment diagram Arc resolution
Placement rule for moment diagrams can be set.

Select any of these options : Model file folder Local system temporary folder Custom Report
Folder for temporary files during analysis
Report language
Depending on your configuration you can select from the following languages: English. Set the amount of virtual memory you let AxisVM use during the analysis here. Italian. You can specify the location of temporary files during analysis. while vibration analysis can be 4 times faster. Improvement depends on the available memory and the model size. Serbian.100
AxisVM 8+Release 4
Analysis
At the beginning of the analysis AxisVM divides the system of equations into blocks according to the available physical and virtual memory. To make the most of this option it is recommended to use a processor with HT-Hyperthread or DualCore technology. Dutch. German. Multi-threading improves speed of calculation.5 times faster. Portugese. Hungarian. Romanian. Spanish. Using a single thread / Using multiple threads Using multiple threads makes AxisVM run analysis on multiple threads. Linear analysis will be 1.
Table layout
. It makes analysis more efficient but can considerably slow down other applications. French. Minimum number of rows per column can be specified to avoid column breaks for short tables. If Allow multiple columns is checked. Russian. narrow report tables will be printed in a multi-column layout to reduce the space required.

the program quits and start the installation of the new release. Click the button to get to the AxisVM Web Update Wizard which is a guide to the download process.15.3 Views
.
3.. searches for program updates.9.3. View
Front view [Ctrl]+ [1] See. If download is complete and the Update the program option is checked on the last page.User’s Manual
101
Update
Search for updates on each startup AxisVM Web Update
If this option is turned on AxisVM searches for live internet connection on each startup.4. 2.
Toolbars to default position
The moveable Icon bar will get back to the left side. All flyout toolbars undocked and dragged to a new position will get back to the Icon bar. If a new release is available it shows a message and let the user download the update.
3. If it finds one..

y.User’s Manual
103
3.) button appears in a line the property can be changed using a separate dialog. FRAC.5. after selecting trusses. SGN. first select all nodes then click the line first line and enter X*2 as X. If result or design tabs are active the values are read only.1. ARCTANH. The question mark button turns on/off the help information. SINH. LOG10.. ). Z or x.
>>
If the (>>) button appears in a line the property can be picked up from another element by clicking it. SIN. ARCTAN.. z. TANH. If the (. Properties are displayed in a tree-like structure. INT. LOG2. Window
3. LN. EXP. ARCSIN. TAN. If the selection contains different elements it is possible to change their common properties (e.5. ROUND. For instance: To scale the structure in direction X by 200%. Few fast operators: ++8 adds 8 to the actual value --8 substracts 8 from the actual value In these expressions # substitutes the actual value (For instance #/3 divide it by 3). In certain fields regular mathematical expressions are also accepted. Property Editor can be used to modify data but also to select and filter elements with the same property. Y. beams and ribs their material and cross-section will be editable). ARCCOSH. COSH. SQRT.g. ABS. elements or loads. ARCSINH. load values. surface thicknesses you can refer to global coordinates as X. Clicking a [+] or [–] symbol before the property name expands or collapses a list of sub-properties. Available operators and functions are: (. ARCCOS. All changes are made immediately. COS.
Property Editor
Property Editor provides the fastest way to change properties of the selected nodes. When entering a value of nodal coordinates.
. SQR.

panning.
Information Windows
Lets you set the display of the Info.5.4. Background pictures are saved into the AXS file.. Picture in the active window can be turned on and off by clicking Display or by [Ctrl+Alt+B].
3.104
AxisVM 8+Release 4
Filter
Selecting a property and clicking the filter button you can select all the elements having the same property value.17 Information Windows
3.5.. rotating and setting the perspective. In multi-window mode each window can have its own background picture.
Background picture
The submenu makes several options available.2. See. 2. Save Background Picture saves the picture in the active window into a file. Example: changing an existing cross-section in the whole structure. Coordinate. submenu item or [Ctrl+B] opens a file browser dialog. Selecting the cross-section property of a rib element you can select all rib elements with this cross-section then change their cross-section property of them.. Remove Background Picture removes the picture in the active window. An automatically fitted background picture can be loaded to the main window of AxisVM to show the model in its future environment.
Split Horizontally
Inactive graphics window
Active graphics window
.
3. Reload Background Picture shows the most recently used picture files. After loading a background picture the model can be set to an appropriate view by zooming out. zooming in.5. and Color Legend Windows to on or off.3.. If the aspect of the picture differs from the window aspect Shift Background Picture makes it possible to drag the background to a new position. Load Background Picture.

5. restoring its view and display settings. Including drawings into a report makes it easier to update the report when the model has changed and recalculated as drawings will be updated automatically like tables. You can maximize or minimize or restore the graphics windows by using the buttons at the top-right of the windows.
3. You can maximize or minimize or restore the graphics windows by using the buttons at the top-right of the windows. The display settings of each window can be set independently. Drawings are not saved pictures but instructions how to draw a view of the model or parts of it including multi-window settings.5. Drawings Library can store displacement.5.
Drawings Library
The Drawings Library contains drawings saved in the program. Drawings can be reloaded to restore saved view and display settings. The display settings of each window can be set independently.5. Different load cases can be set in each window but only when displaying results. reinforced concrete column check and beam design in an associative way. stress diagrams of line elements. force. Clicking the arrow beside the tool button an existing drawing can be selected from a popup list. punching analysis. diagrams of steel and bolted joint design.
3.
3.
Close Window
Closes the current graphics window.7.
Split Vertically
Active graphics window
Inactive graphics window
Inactive graphics window
Splits the graphics window vertically into two parts.6.User’s Manual
105
Splits the graphics window horizontally into two parts.
.

Restore result components If this option is checked loading a drawing displaying results restores the result component as well and sets the appropriate tab (Static. Vibration.
This dialog is to overview. OK Cancel Saves the changes and loads the selected drawing. maintain and relaod saved drawings.106
AxisVM 8+Release 4
After clicking the Drawings Library tool button a dialog appears. (available in multi-window mode only) Loads a chosen drawing to the window.5.8.
3. If this option is unchecked loading a drawing does not restore the result component and the tab.
Save to Drawings Library
. Deletes a drawing from the Drawings Library Loads a chosen drawing to the active window. Does not save changes. etc.).

About
Tells you more information about your AxisVM program.. See.6.6. load combinations (and result components if results are displayed) can be chosen.User’s Manual
107
By clicking this tool button one or more drawings can be saved into the Drawings Library. If the current drawing is.
3.5.
Contents
[F1] Opens the table of contents of the help.2.
Latest release information and history of fixes and new developments. AxisVM creates all combinations (i.
3.3.
3..6. To get context-sensitive help information about the operations related to a dialog box press [F1].3. It can be overwritten or the drawing can be renamed.
3.1. all selected result components in all selected load cases) and saves them into the Drawings Library with the current view and display settings. Multiple drawings button opens additional options.
AxisVM Home Page
Visits AxisVM Home Page using the default Internet browser.
.
AxisVM Update
Launches the AxisVM Web Update Wizard. Load cases.4. 3.
Release information. serial number and time limit of your AxisVM version. You can use this command to determine the version/release number. Clicking the Drawings Library button displays the Dawings Library dialog.6.6. a Found in the Drawings Library label is displayed in the dialog.. and allows access to the topics you are interested in.e.6.. Help
Lets you use the online help of AxisVM.8 Preferences
3.
3. configuration.

Geometry
Geometry commands let you interactively and graphically create the model geometry in 3D. The model geometry is defined by nodes (points). mesh lines (lines) between nodes. and surfaces (triangular or quadrilateral) created from three or four appropriate lines. and load case/combination definition). or shells) the mesh consists of quadrilaterals that represent the median plane of the elements.
The Preprocessor
The preprocessor lets you create or modify the geometry of the model.
4. This chapter introduces the AxisVM modeling commands (geometry generation. element/mesh generation. in a completely visual way.User’s Manual
111
4. membranes.
. Later you can define finite elements based on the geometry constructed here. Automatic meshing on domains Automatic meshing on macro quads and triangles
In the case of frame structures (beams or trusses) the mesh consists of the axes of the elements. In the case of surface structures (plates. The advanced Visual Modeling feature allows quick and reliable modeling and design.1.

When AxisVM starts, the graphical user interface is ready for geometry editing. In case of a new model X-Y, X-Z or perspective view can be set as the default view. In case of an existing model the latest view settings will be loaded. Using the horizontal icon toolbar at the top of the graphics area you can apply various commands to construct geometry meshes describing the geometry of your finite element model. See...4.8 Geometry Toolbar Using the vertical icon bar on the left you can apply commands that change the display of the model, and can configure the working environment of the editor. See...2.15 The Icon

4.2.1.

Multi-Window Mode
When the model is complex, it is useful to display different views of the model simultaneously on the screen. AxisVM allows you to split the graphics area horizontally or vertically. Each newly created graphics window has its own settings, and allows the independent display of the model views. This feature is also useful when interpreting results. You can access split commands from the Window menu.

Split horizontally

Splits the active graphics window horizontally into two equal parts. The top window will become the active window. See... 3.5.4 Split Horizontally

Split vertically

Splits the active graphics window vertically into two equal parts. The left window will become the active window. See... 3.5.5 Split Vertically

Close Window

Closes the active window if there are more than one graphics windows in use. The new default window will be that in which you previously worked. You can change views during any editing command.

F

In the perspective view some editing commands cannot be used, or are limited in use.

User’s Manual

113

4.3. Coordinate Systems
AxisVM uses different coordinate systems, to describe the model. The global coordinate system is used to describe the model geometry. Local coordinate systems are mainly used in the element definitions. The local systems are usually defined by the element geometry and additional references. AxisVM denotes the axes of the global system with capital letters, and the local axes with small letters. The geometry can be created using Cartesian, Cylindrical or Spherical coordinate systems. See... 4.3.2. Polar Coordinates

4.3.1.

Cartesian Coordinate System
AxisVM uses Cartesian coordinates to store geometry data. AxisVM uses the right-hand rule exclusively to define the positive directions of axes and rotation. The illustration below shows the positive directions of the axes and of rotation according to the right-hand rule.

Base coordinate system

Global and relative origo

A new model uses the view selected in the New Model dialog (see... 3.1.1 New Model). The origin of the coordinate system is shown by a blue X initially located at the left bottom corner of the editor window. A fixed (X, Y, Z) and a relative (dX, dY, dZ) global system are used to locate points (nodes) in your model. The origin of the relative system can be moved anywhere (using [Alt]+[Shift] or [Insert]), at any time during modeling. The Coordinate Window displays either the fixed or the relative global coordinates according to its current settings. If the relative mode is selected, the denotation of axes becomes dX, dY, dZ. With the help of the Coordinate Window, and according to the movement of the relative origin you can make measurements on the model (distances, angles). The nodal displacements and mode shapes refer to the fixed global system. In the X-Y and Y-Z views the third axis (normal to the view’s plane) is oriented toward you. As a result, when a copy is made by translation with a positive increment about the respective third axis, the copies will be placed in front (toward you). The opposite occurs with the third axis in the case of an X-Z view is oriented in the opposite direction. See...4.9.17 References

F

114

AxisVM 8+Release 4

4.3.2.

Polar Coordinates
In addition to the Cartesian global coordinate system, you can use either a cylindrical or a spherical coordinate system. One of the polar coordinate systems can be selected through its corresponding radio button in Settings / Options / Editing / Polar coordinates. In the Coordinate Window three variables will be displayed depending on selection: Cylindrical h: the value measured from the view plane to a point on the cylinder’s main axis (that is perpendicular to the view plane) oriented outward from the screen r: radius that is the distance on the view plane from the projection of the point to the cylinder’s main axis a: the angle between the line that joins the point with the origin and the horizontal Spherical r: the radius, that is the distance from the point to the sphere’s center (origin) a: the angle on the view plane between the line that joins the projection of the point with the origin and the horizontal b: the angle between the line that joins the point with the origin and the view plane, which is positive if the point is in front of the view plane (between the user and the view plane).

Cylindrical Coordinate System

Spherical Coordinate System

4.4. Coordinate Window

Displays the current absolute and relative values of the cursor position in the global coordinate system (Cartesian and cylindrical or spherical). You can switch between absolute and relative coordinate displays, by clicking on the letters d in the Coordinate Window. The display of the d letters also show whether the relative coordinates are enabled or not.

The positive angles, α:

F

The relative switch (delta) can be used together with the constrained cursor movements. See... 4.7.4 Constrained Cursor Movements.

User’s Manual

115

4.5. Grid
See in detail...2.15.14.1 Options

4.6. Cursor Step
See in detail...2.15.14.1 Options

4.7. Editing Tools
Editing tools help the work by several features. See... 2.15.14.2 Editing

4.7.1.

Cursor Identification
Sets the size of the cursor identification area (in pixels). When you position the cursor over the graphics area, AxisVM finds the entity of the model that is closest to the center of the cursor from among the entities that are located in or intersect the identification area. The size of the identification area can be set at Settings / Options / Editing / Cursor identification. The current shape of the cursor shows what kind of entity was identified. Depending on entity type, the cursor will have the following shapes: Node Mid-side node Support Edge hinge Mesh independent load Load polygon vertex Center of an arc Arc Tangent References Line Surface Intersection Perpendicular (normal) Guideline Domain

116

AxisVM 8+Release 4

Rigid element Dimension line In case of Pick up function Text box, label If there are several entities at the same location, the program identifies the first entity according to the ordering of the list above. If there are multiple entities of the same type, the cursor will show a double symbol.

F
Background detection

Use the Coordinate Window to find out which one of the elements was actually identified. The cursor can be set to detect the lines on architecture background layers.

4.7.2.

Entering Coordinates Numerically
During the model editing, coordinates of the cursor can be specified directly entering the numerical values into the Coordinate Window. There are two ways to enter the numerical values: 1. by pressing the corresponding character button on the keyboard 2. by clicking with the left 8 button on the desired coordinate value display field, and then typing in the value. If the relative mode is enabled (the letter d is depressed), the coordinates you enter will define a point from the relative origin. If contradictory values are entered (in case of a constraint), the last entered value will update the others. The relative origin can be moved at any time, anywhere. Therefore when drawing a line, you can specify its endpoint coordinates relative to different origins.

F

To draw a line with a given length and direction move to relative origin to the starting point, enter the angle at d a[°] and enter the length at d r[m] then press the Enter button.

4.7.3.

Measuring Distance
The distance between two points or the length of a line can be measured by moving the relative origin onto the first point and then identifying the second point by positioning the cursor over it. In this case the value of dL in the Coordinate Window is the distance between the points. The cursor can be moved to a location relative to a reference point by moving the relative origin onto the reference point, then entering the angle in the input field da and the distance in the dr input field.

4.7.4.

Constrained Cursor Movements
The cursor movement constraints can be customized in the Settings / Options / Editing dialog. The constrained cursor movements use the following values:

User’s Manual

117

∆α

Holding the [Shift] key pressed, the cursor is moving along a line that connects its current position with the origin, and that has an n*∆α angle, where the value of n depends on the current cursor position. Holding the [Shift] key pressed, the cursor is moved a line that connects its current position with the origin, and that has an α or α+n*90° angle, where the value of n depends on the current cursor position. ∆α and α can be set in Settings/Options/Editing/Constraint Angle. The meaning of origin depends on the d switches of the coordinate palette. Turning off both the origin will be the global origin. Turning on any of the d switches the origin will be the local origin.

Custom α

n × ∆α custom α+90 ο custom α

F

You cannot use ∆α and Custom α constraints in perspective view. If the cursor is over a line, holding the key [Shift] depressed, will constrain the cursor movement to the line and its extension . If the cursor identifies a point, holding the key [Shift] depressed, makes the cursor move along the line defined by the point and the relative origin..

Constraint

When the cursor identifies a domain or surface element pressing [Shift] makes the cursor move in the plane of the element.

Intersection point

Node

Perpendicular Midside point

surfaces will be divided into smaller surfaces if necessary.. A frozen coordinate will not change on cursor motion.[Z]. allowing for better positioning.[A].[R]. [H] respectively. Set the line intersection options in Settings/Options/Editing/ Auto Intersect. and the resulting elements will have the same material and cross-sectional properties as the original.
.6.15. they will be split.14.[Y].2 Editing If Auto Intersection is on. 2. Surface finite elements are also divided and the new elements inherit the properties and loads of the original element.
Freezing Coordinates
You can freeze the value of a coordinate..8 Geometry Tools
4.118
AxisVM 8+Release 4
Geometry Tools The icons of Geometry Tools allow you to lock the direction of drawing a line. that was used to freeze it or press [Alt]+ [Space]. If surfaces are intersected by lines.7.[B]. Freezing can be achieved by using [Alt] + [X]. To cancel coordinate freezing. a node will be generated and the lines will be bisected.15. See.
Frozen X coordinate
Frozen angle
4.5.
Auto Intersect
At the intersection point of the lines.7. press the same button combination.[L]. See. A black rectangle over the coordinate input field shows that the coordinate is frozen.. 2..

2.. [Esc] key 2. When working on parts with Settings / Options / Editing / Auto / Part Management turned on all geometric entities created will be automatically added to the active parts.
4. 3. To place a node: 1.
F
If you are working on parts and Settings / Options / Editing / Auto / Part Management option is checked then all the newly created geometric entities will be added to the active parts. The line type can be chosen by clicking on the arrow at the bottom-right corner of the currently used Line Tool Icon. otherwise it remains independent of the line. You must specify the vertices. [Esc] key a second time will exit polyline drawing mode.2. and then press [Space] or [Enter] (it works in all views). To draw lines in perspective in a different plane workplanes can be used. You can place a node on a line or surface. Geometry Toolbar
These tool buttons create new geometry or change the existing one. the line or surface will be divided by the new node. You can cancel the process by pressing the [Esc] key or the right mouse button.8. The command lets you generate one or more independent lines. The geometric entities can be selected prior to applying the geometry construction commands. 8 right button & Quick Menu/Cancel 4. nodes will be merged.
4. If the Settings / Options / Editing / Auto Intersect check-box is enabled.
Polyline
.User’s Manual
119
4. You must graphically or numerically (by the Coordinate Window) specify the endpoints (nodes). The Line Tool offers the following options to draw simple shapes: Line Constructs straight lines by defining their end points (nodes). See. 8 left button while pointing to the last point (node) of the current polyline. as well.
Node (Point)
Lets you place new nodes or modify existing ones. 0 Workplanes.8. Exit current polyline by pressing the: 1.
Line
The Line Tool is to construct lines or other simple shapes. Move the graphics cursor to the desired location and press the [Space] key or the left mouse button (in perspective view you can place nodes only to special locations). In perspective view lines are drawn on the Z=0 plane by default. Constructs a series of connected straight lines (a polyline).
F
If nodes are generated closer to each other than the tolerance specified in Settings / Options / Editing / Editing Tolerance value.. and then clicking on the desired Line Icon.. Enter the node coordinates numerically in the Coordinate Window.8.1.

Skewed rectangle Constructs a skewed rectangle (its corner points (nodes) and edge lines). you can draw skewed rectangles using only the existing points. Arcs and circles will be displayed as polygons according to the Arc resolution set in Settings / Preferences / Display.
Arc
Draws an arc or a circle.8. You must specify one of its sides (by its endpoints).
2nd point
3rd point
arc
1st point (central point)
Defining an arc by three points.
4. This command is not available in perspective view. Polygon Number of sides has to be defined in a dialog. [Esc] cancels the command.
After you specified the first corner you can cancel the command by pressing the [Esc] key.120
AxisVM 8+Release 4
Rectangle
Constructs a rectangle (its corner points (nodes) and edge lines). The command can be applied in perspective setting as well. In perspective view.
After you specify the first corner you can cancel the command pressing the [Esc] key. You must specify two opposite corner points.
2nd point 3rd point arc
1st point
Endpoint
. Polygon has to be defined by entering a centerpoint and 2 polygon points. Defining an arc by its radius. and then the other side. and starting and ending points.3.

If finite elements are intersected new elements inherit properties and loads of the original element. it can be used directly as a finite element mesh. You must successively graphically select the corners (four points).
Vertical Division
This function creates a horizontal divider line passing through the cursor position.
$
The quad and the mesh are displayed with solid grey lines. or with any side lines). This line is in a plane parallel with the X-Y.6.
Quad-to-quads
Generates an n×m mesh between the corners of a 3D quad (not necessarily flat.
. Creates new nodes at the intersections. X-Z or Y-Z plane depending on the actual view (or parallel with the workplane if a workplane is used). the quad is displayed with red dotted lines. If finite elements are intersected new elements inherit properties and loads of the original element.
4.8.8. Creates new nodes at the intersections. If a quad shape is entered that is not allowed (e. and the number of segments ( N 2 ≥ 1 ) between corners 2 and 3. concave). X-Z or Y-Z plane depending on the actual view (or parallel with the workplane if a workplane is used). Use this command to generate a macro mesh before applying a finite element mesh generation command. If the mesh is fine enough.
Quad/Triangle Division
Constructs a mesh of quads/triangles over a quad or triangle.8.
Horizontal Division
This function creates a horizontal divider line passing through the cursor position.User’s Manual
121
4.4. and specify the number of segments ( N 1 ≥ 1 ) between corners 1 and 2.g. This line is in a plane parallel with the X-Y. the quad is displayed with grey dotted lines.5. If the mesh leads to quad subdivisions that are distorted (have an angle smaller than 30° or greater than 150°).
4.

If the mesh leads to triangle subdivisions that are distorted (have an angle smaller than 15° or greater than 165°). The quad and the mesh is displayed with solid grey lines. or to triangle subdivisions that are too distorted (has an angle smaller than 15º or greater than 165º). If the mesh leads to quad subdivisions that are distorted (have an angle smaller than 30º or greater than 150º). The triangle and the mesh are displayed with solid grey lines. three collinear corners). and specify the number of segments N between corners. concave). the quad is displayed with red dotted lines. the triangle is displayed with grey dotted lines.g. If a quad shape is entered that is not allowed (e. except that each generated quad is divided into two triangles by its diagonals which are parallel to the side first entered. If a quad shape is entered that is not allowed (e. the quad is displayed with grey dotted lines.122
AxisVM 8+Release 4
Quad-to-triangles
$
The command is similar to the quad-toquads command.
. but each generated quad is divided into two triangles by its shorter diagonal. The mesh will also contain triangles along the side that corresponds to the first two corners entered. You must graphically select the corners successively (three points).
$
Triangle-to-triangle
The command is similar to the triangle-toquads command.g.
$
Same as for triangle-to-quads. the triangle is displayed with red dotted lines.
Triangle-to-quads
Constructs a mesh between the corners of a triangle (not necessarily with any side lines).

. By Length: Lets you divide the selected lines into two segments.
before division
after division
If finite elements are divided the new elements inherit properties and loads of the original elements.9. a=0. You must specify the length (d) of the segment corresponding to the first node (i end). using this command you can intersect the selected lines.
F
If you divide surface edge lines surface elements will be deleted. Evenly: Lets you divide the selected lines into several equal-length segments.
4.User’s Manual
123
4.
Normal Transversal
Creates a connection between to lines along their normal tranversal.
4. You must specify the length of segments (d).8.7. The following input options are available: By Ratio: Lets you divide the selected lines into two segments. You must specify the parameter a of the location of the inserted node relative to the first node (i). You must specify the number of segments (N).8. The parameter d must be between 0 and the total length). finite elements are also divided and inherit the properties and loads of the original element.
Line Division
Lets you create new point (nodes) on the selected lines. The parameter a must be between 0 and 1.
Intersect
Divides the selected lines by creating nodes (points) at their intersections.8.5 represents a division of the selected lines into two equal segments. Uniform by length: Lets you divide the selected lines into several equal-length segments.
.8. You can select elements for intersection beforehand.
F
If the Settings / Options / Editing / Auto / Intersect check-box was not enabled in the dialog window at the time of creating the geometric entity. If finite elements are assigned to the lines.

.8. The number of surfaces detected is displayed in an info dialog.8.
Select unattached nodes or lines: If this check-box is enabled.8. You can specify the maximum tolerance (distance) for merging points. Domain Intersection
Creates intersection lines of domains and line elements.11.10.
4.
Points that are closer together than this distance are considered to be coinciding. The mesh then can be refined. The reported surfaces are geometry surfaces but not surface elements. membranes. The coordinates of the merged points (nodes) are averaged.
4. or shells) you have to create a mesh that consists of triangles and convex flat quadrilaterals. Geometry Check
This function eliminates extra nodes and lines within a given tolerance. The default value is ∆L=0.12. After clicking the tool button select domains to create their intersection or select a domain and a line to create the intersection. AxisVM will send a warning message if unattached (independent) parts are encountered. To avoid having hiding lines check Settings / Options / Editing / Auto / Intersect or click Intersect on the Geometry Toolbar. You must select all surface edges when applying the command.001 [m]. Surface
In any cases when you wish to model surfaces (plates. You can make them surface elements by assigning material and cross-section properties to them. The command searches all triangles and quads in the selected mesh of lines.124
AxisVM 8+Release 4
4. The command reports the number of merged nodes/lines.
F
The following case is not identified by the Check command.

3. Click on any of the selected nodes. AxisVM takes into account only those surfaces that have an out-of-plane measurement smaller that the tolerance entered in the Settings / Options / Editing / Editing Tolerance. Drag the node/line/surface to its new position.User’s Manual
125
F
Quads have to be flat. Fast modify: Clicking a node you get to the Table Browser where you can enter new coordinate values. Position the cursor over the node/line/centre of surface. the position of all nodes and lines will be modified.
F
If multiple nodes and/or lines are selected.8. 3. 2. drag the node/line/surface. transform
Lets you modify existing geometric entities. To modify nodes or lines: 1. Holding the left mouse button pressed. 2. Moving selected nodes into the same plane: If the plane is a global one you can move selected nodes into this plane easily. all the selected nodes will appear in the table. Their position can be set in Settings / Preferences / Toolbar. Modify.13. Use Edit / Set common value to set a common coordinate value.
Set palette while nodes are moved
. or enter its new coordinates in the Coordinate Window.
Using pet palettes
Depending on the type of the dragged element different pet palettes appear on the screen. and then press enter or press the left mouse button again.
4. Select the entire column of the respective coordinate. If multiple nodes are selected and you click one of them. 1.

Dragging the node. Dragging the arc parallel with its original position. Entering node coordinates: Clicking a node the table of nodes appears where coordinates can be changed. Select nodes to align.. 3.. Enter the required coordinate value in the property editor. 4. Inflating / deflating the arc. In the definition process you must define and assign different property sets. 2. 3. Straightening the arc. 3. Dragging the node lengthening or shortening connecting arcs. See the last two tool buttons in Dragging nodes.
The commands associated with the icons let you define the finite elements used for modeling. Transforming objects See.
.5 Delete
4. 3.126
AxisVM 8+Release 4
Dragging nodes The following dragging modes can be selected: 1. Delete
[Del] See in detail. Examples of aligning nodes to a plane if this plane is parallel with one of the global coordinate plane: 1.14. 2. the startpoint and midpoint of the original arc.5 Geometric tranformations on objects
4. Dragging the node disconnecting selected connecting lines. Center angle remains constant. The new arc is defined by the dragged node.15. Dragging the line parallel with its original position. Breaking the line at a given point by adding a node.. Changing radius of the arc.2. 1. 2. See the last two tool buttons in Dragging nodes. The last two tool buttons determines the behaviour of connecting arcs. Making an arc.8. After selecting one or more nodes their coordinates can be edited in the property editor as well. 4. 2. Dragging lines The following dragging modes can be selected: 1.. 2. 2.9. Finite Elements
The commands related to the definition of the finite elements are described below. Dragging arcs The following dragging modes can be selected: 1. Dragging the node translating connecting lines.

The following parameters are stored:
F
If a material type is deleted all elements made of this material will be deleted. If you delete a material property set. SIA and other specifications. DIN.9.
.User’s Manual
127
Depending on the type of finite element.
F
Browse Material Library [Ctrl+L]
AxisVM uses exclusively isotropic materials with linear elastic behavior.1. the definition of the elements with the respective material will be deleted. and the active or inactive stiffness depending on its initial opening for the gap element. you have to define the following properties: Properties of finite elements
Finite element Material Crosssection Reference Stiffness Surface
Truss Beam Rib Membrane Plate Shell Support Rigid Spring Gap Link Edge hinge o: optional
• • • • • •
• • •
o • o • • • • o
o • • • • • • • •
Note that some elements like springs and gaps can have nonlinear elastic stiffness properties that are taken into account only in a nonlinear analysis.
4. In a linear analysis the initial stiffness is taken into account for the spring element. NEN. The material library contains material properties of civil engineering materials based on Eurocode.
Material
Define Materials
Lets you define and save material property sets or load them from a material library.

spring elements). The beam. The properties are related to the element’s local coordinate system. membrane. You must enter values for all properties. and shell elements). Cross section properties are defined in the coordinate system of a truss / beam / rib element. link.
.. and uniform isotropic or orthotropic (for beam. rib.128
AxisVM 8+Release 4
Material Properties
Depending on the type of the finite element you must define the following material properties: Finite Element Truss Beam Rib Membrane Plate Shell Support Rigid Spring Gap Link E • • • • • • n a • • • • • • r • • • • • •
• • •
Displaying and changing material properties is described in 3.13 Cross-Section Library
F
If you delete a cross-section property set.
Cross-Section
Define Crosssections
Lets you define and save cross-sectional property sets or load them from a cross-section library. or stiffness (support. and rib elements require a cross-section.
F
In AxisVM all the materials are considered to be linear elastic (Hooke’s Law). truss. The lines will not be deleted.
4. For cross-section properties see.1.2. In a linear analysis the initial stiffness is taken into account for the nonlinear elements..12 Material Library.1. 3. the definition of the elements to which it was assigned will also be deleted. Some elements can have nonlinear elastic material (truss). gap.9. plate. Nonlinear material models are taken into account only in a nonlinear analysis.

. internal lines and points of a domain: point. The domain can be meshed automatically. 4. Polygon vertices. See. and surface support rib element distributed load dead load thermal load nodal degrees of freedom (DOF)
$
A domain is displayed by a contour line inside of the domain’s polygon.3. holes and internal lines must be in same plane. A domain can contain holes.
.2 Mesh generation on domain More than one domain can be used to model a structural element.11. A domain has the following parameters: Element type (membrane. with a color corresponding to the domain’s element type (blue for membrane.
Domains can be defined for floors. and green for shell). and any other complex structural surface element. plate.User’s Manual
129
4.9.. shell) Material Thickness Local coordinate system The following parameters can be assigned to the polygon. walls. internal lines and points. line.
Domain
A domain is a planar structural element with a complex geometric shape described by a closed polygon made of lines and arcs.1. hole edges. red for plate.
2nd domain
1st Domain
1st domain
3rd domain
A domain can contain other (sub-) domains.

You can move holes from one domain to another. The program applies the parameters you entered in a dialog window. or change their shape. Select the (closed) polygons that are the edges of the holes you want to define. Holes have to be inside the domain and in the domain’s plane.
Hole
Holes can be defined in domains.4.
4. select the domains (click on the contour line of the domain) you want to delete and click OK in the dialog. AxisVM will find the planes and the contour polygons of the set.
Domain
1st Hole
$
Holes are displayed by a contour line with the color of the domain in which they are located. If you select more lines or lines from different planes.
Modify a domain Delete a domain
Select the domain (click on the contour line of the domain) you want to modify and make the changes in the dialog displayed.
.130
AxisVM 8+Release 4
Define a domain
Select lines on the contour of the domains you want to define.9. Press the [Del] button.

local system) will be retained but the existing mesh will be removed. Change selection to modify domain contour and click OK on the selectioin toolbar. Click the Change domain contour icon on the toolbar.
Change domain contour
1. Select the domains and click OK on the selection toolbar. Select the cutting line and click OK on the selection toolbar.User’s Manual
131
4. cut and a union of domains can be calculated.
Before
After
. thickness. Domain countour will be selected. Click the Cut of a domain icon on the toolbar. 3. 1. local system). material.
Before
After
F
Domain properties (material. Click the Union of domains icon on the toolbar. 2. Select a domain to change.
Domain operations
Domain contours can be changed. 3.5. 2.
Before Cut a domain
After
To cut a domain along en existing line: 1.9. loads will automatically be removed. 2.
Union of Domains
Union can be created from adjacent domains with matching properties (same thickness. If loaded areas are removed from the domain. Select the domain.

.132
AxisVM 8+Release 4
4.11 Break apart structural members
Truss
Browse Material Library Cross-section Editor Browse Cross-Section Library
Truss elements can be used to model truss structures. Line elements are handled as structural members and not as finite elements. 3.
Line Elements
Line elements are defined and modified in a common dialog. The cross-section selected will be added to the cross-section table of the model. A maximum of three translational degrees of freedom are defined for each node of the elements.2. The cross-section created in the Editor will be registered in the list of model cross-sections. listing functions will consider it to be a single structural member. Meshing a line element divides a beam or a rib into finite elements. Trusses are two node. labeling. Allows browsing of the cross-section library to assign a cross-section to the element. Numbering. The variation of the axial force is constant along the element. i denotes the truss end with the lower node index (first node). straight elements with constant cross-section properties along the truss length. Structural members can be broken apart by Edit / Break apart structural members) See. It can be changed by selecting the other orientation from Local x Orientation. By default the element x axis goes from the node (i). If elements of different type are selected element definition will be activated. Allows browsing of the material library to assign a material to the element. Axial internal forces Nx are calculated for each truss.6. Define You must select the lines to which you want to assign the same material and cross-sectional properties in order to define truss elements.10 Find structural members.2. The material selected will be added to the material table of the model. Materials and cross-sections can be selected from built-in libraries or from a list of the materials/cross-sections already defined.
Defining materials and cross-sections
. (Edit / Find structural members). to the node (j).. 3. Launches the Cross-section Editor. Existing line elements can be joined to form a single element if the geometry and their properties allow it.9. After choosing the element type specific truss / beam / rib element parameters can be set. The elements are pin-ended (spherical hinges).

or buckling analysis is performed. The variation of the internal forces along the beam are: constant axial force. In any other case the angle is relative to the global Z axis.User’s Manual
133
$
Local x Orientation
The truss elements are displayed on the screen as red lines. Three orthogonal internal forces. Automatic orientation is based on the endpoint coordinates i à j : local x axis is directed from the end node with a lower number to the node with the higher one j à i : local x axis is directed from the end node with a higher number to the node with the lower one Cross-section: In the calculation of the element stiffness. The options are: from i to j or from j to i or automaticaly. The automatic local coordinate system (and the cross-section) can be rotated around the element axis by a custom angle.. and three internal moments. This allows a correct display of the cross-section on the screen. straight elements with constant or variable (linearly changing) cross-section properties along the beam length. 4.9. In a nonlinear analysis you can specify that a truss has stiffness only if it is in tension or compression. Affects only the display of references. A reference point can be assigned to define the element orientation. My. one axial and two shear (Nx. You can optionally enter a resistance value as well. If the element is parallel with the global Z direction. Beams are two-node.
. vibration. constant torsion. See. one torsional and two flexural (Tx. A reference point is used to arbitrarily orient the element in 3-dimensional space (to define the local x-z plane). Local orientation of the beam can be changed. V y. The initial elastic stiffness of a truss element is taken into account if a linear static. A maximum of three translational and three rotational degrees of freedom are defined for each node of the elements. only the cross-sectional area Ax is considered from the cross-sectional properties. A nonlinear elastic behavior is assumed for the nonlinear truss elements. disregarding any nonlinear parameter entered.. the angle is relative to the global X axis. The ends of the elements can have arbitrary releases. In case of selecting Auto the reference(s) will be set by the program. Mz) are calculated at each cross-section of each element. The displacements and internal forces are calculated at intervals of at least 1/10 of the element length. V z).17 References Rotation of cross-sections is made easy by the reference angle. The nonlinear parameters are taken into account only in a nonlinear analysis.
Local z Reference
Reference angle
Nonlinear parameters
F
Beam
Beam elements may be used to model frame structures. constant shear forces and linear moments.

the angle is relative to the global X axis.
$
End releases
End releases at the start node
End releases at the end node
˜
Graphical symbol of a rigid connection code (the corresponding local displacement component of the beam end is transferred to the node) Graphical symbol of a hinged connection code (the corresponding local displacement component of the beam end is not transferred to the node) Graphical symbol of a semi-rigid connection code (the corresponding local displacement component of the beam end is partially transferred to the node) Graphical symbol of a plastic connection: the maximum value of the moment at the endpoints is calculated from the material and cross-section properties. Each code corresponds to one internal force component.17 References. In any other case the angle is relative to the global Z axis. The automatic local coordinate system (and the cross-section) can be rotated around the element axis by a custom angle. local x orientation Automatic reference
Defining material.9.
Reference point
Material. The end-releases are set by a six code set for each end. By default the beam ends are considered rigidly connected (all codes are of rigid connection) to the nodes. cross-section and local direction X are similar to truss elements. The beam elements are displayed on the screen as blue lines. If the element is parallel with the global Z direction. Setting a code as hinged connection will result in the corresponding internal force component of the respective end to be released. The reference vector will be generated by the program according to the section 4. to the node (j).
Reference angle
Rotation of cross-sections is made easy by the reference angle. It can be changed by selecting the other orientation from Local x Orientation.134
AxisVM 8+Release 4
i denotes the beam end with the lower node index (first node). crosssection. You can specify releases that remove the connection between the selected elements’ degrees of freedom (in the local coordinate system) and the nodes. The orientation of the local x axis of the element can be reversed or can be set to Auto which means that local x directions will be set automatically based on the beam end coordinates. A semi-rigid connection code can be assigned to the in-plane rotation components of the beam ends.
. By default the element x axis goes from the node (i).

Connection: Model:
Moment . j end numerical code: 000111).Relative Rotation Diagram
. the initial stiffness of the connection is taken into account. a rigid body rotation about element axis is introduced. Can’t transmit Mz and My moments. and M z moments. The value should be the initial stiffness of the real connection M-φ characteristics. or buckling analysis. Hinge in x-z plane. For example. Can’t transmit Mz moment. My. Free translation along local y axis.User’s Manual
135
The table below demonstrates the use of end releases for some common cases: End Release Hinge in x-y plane. vibration. Can’t transmit My moment.g. In a linear static.relative rotation diagram of a connection is modeled by a linear or nonlinear elastic rotational spring. Example: Start node End node
Semi-rigid connection
To define semi-rigid hinges set the radio button to semi-rigid and enter the torsional stiffness of the linear elastic spring modeling the connection about the local axis y or z. Free translation along local z axis. if you specify spherical hinges at both ends (code: 000111). Can’t transmit Vy shear force. Hinge in x-y and x-z plane. Symbol
F
Care must be taken not to release an element or group of elements such that rigid body translations or rotations are introduced. i end numerical code: 000011. Can’t transmit Vz shear force. The moment . The nonlinear characteristic can be used only in a nonlinear static analysis. In this case at one of the ends you may not release the element degree of freedom corresponding to the rotation about local x axis (e. Can’t transmit Mx. Hinge in x-y and x-z plane and free rotation about local x axis (spherical hinge).

136

AxisVM 8+Release 4

F
Moment Resistance

For example, in the case of steel frame structures, Eurocode 3 Annex J gives the details of application. To fixed or semi-rigid connections a moment resistance can be assigned, that is the maximum moment that can develop in the connection. The moment resistance parameter is used only in case of a non-linear analysis. To define plastic hinges set the radio button to plastic. Moment resistance will be displayed but cannot be edited. If elements with different materials or crosssections are selected no value will appear in the edit field but hinges will be defined with the appropriate moment resistance. Plastic hinges can only be used with steel beams. If any beam end release code is of a hinged connection, the beam end is displayed on the screen as a blue circle. If it has a stiffness value a blue cross is inscribed. If the end release corresponds to a spherical hinge, it is displayed as a red circle. The plastic hinges are displayed as solid circles. The defined beams appear as dark blue lines.

F
Plastic hinge

F $

Rib

Rib elements may be used, independently or in conjunction with surface elements (plates, membranes, and shells) to model ribbed surface structures. When used attached to surface elements, the ribs can be connected centrically or eccentrically to the surface elements. The properties of the corresponding surface elements are used to orient the element in the 3-dimensional space (to define the local x-z plane). When used independently, the ribs can model frame structures in a similar way as the beam element, but it can take into account the shear deformations. A reference point or vector is required to arbitrarily orient the element in the 3D space. Rib elements are isoparametric three node, straight elements with constant or variable (linearly changing) cross-section properties along the rib length, and with quadratic interpolation functions. Three translational and three rotational degrees of freedom are defined for the nodes of the element. Three orthogonal internal forces, one axial and two shear (Nx, V y, V z), and three internal moments, one torsional and two flexural (Tx, My, Mz) are calculated at each node of each element. The variation of the internal forces within an element can be regarded as linear.

You must assign the following properties: Defining material, cross-section and local direction X are similar to truss elements. The material of the rib can be different from the surface material (if it is connected to a surface). The rib element’s cross-section is taken into account as is shown in the figure below: The reference vector will be generated by the program according to the section References Independent rib: The local coordinate system is defined as follows: the element axis defines the x local axis; the local z axis is defined by the reference point or vector; the y local axis is according to the right-hand rule.
Reference point

Rib connected to a surface element: The local coordinate system is defined as follows: the element axis defines the x local axis; the local z axis is parallel with the z axis of the surface element; the y local axis is parallel with the plane of the surface element, oriented according to the right-hand rule. The figure below shows that when the beam is located on the edge of two surface elements that makes an angle, the local z axis is oriented by the average of normal axes of the surfaces. If more than two surfaces are connected to the edge and you select one or two of them then an automatic reference will be available when defining the rib. The cross-sectional properties must be defined in this coordinate system.
Reference point

Reference angle

The automatic local coordinate system (and the cross-section) can be rotated around the element axis by a custom angle. If the element is parallel with the global Z direction, the angle is relative to the global X axis. In any other case the angle is relative to the global Z axis. End releases can be defined for ribs the same way as for beams. By default both ends are fixed. You can specify eccentricity for a rib only if it is on the edge of one or two surfaces. If more than two surfaces are connected to the edge and you select one or two of them you can define eccentricity for the rib. The eccentricity (ecc) of a rib is given by the distance of the center of gravity of its cross-section to the plane of the model of the surface (neutral plane). It is positive if the center of gravity is on the positive direction of its local z axis.

End releases Eccentricity

138

AxisVM 8+Release 4

F

For plates, the eccentricity of the rib will modify the flexural inertia of the rib as follows:
I * = I y + A * exc 2 y

For shells, due to the eccentric connection of the rib to the shell, axial forces will appear in the rib and shell.

$
Modifying

Ribs appear as blue lines. Selecting elements of the same type and clicking the tool button Modifying will be actived. Properties of elements can be changed if the checkbox before the value is checked. If a certain property is does not have a common value its edit field will be empty. If a value is entered it will be assigned to all selected elements. Properties of another element can be picked up and assigned to the selected elements. Clicking the Pick Up button closes the dialog. Clicking an element picks up the value and shows the dialog again. Only those properties will be copied where the checkbox is checked.

Pick Up>>

4.9.7.

Surface Elements
Surface elements can be used to model membranes (membrane element), thin and thick plates (plate element) and shells (shell element) assuming that the displacements are small. As surface elements you can use a six node triangular or eight/nine node quadrilateral finite elements, formulated in an isoparametric approach. The surface elements are flat and have constant thickness within the elements.

F

It is preferable for the element thickness not to exceed the (1/10)th of the smallest characteristic size of the modeled structural element, and the deflection (w) of a plate or shell structural element is less than 20% of its thickness (displacements are small compared to the plate thickness). Use of elements with the ratio of the longest to shortest element side lengths larger than 5, or with the ratio of the longest structural element side length to the thickness larger than 100 are not recommended In some cases when the elements are used (that are flat with straight edges) to approximate curved surfaces or boundaries, poor results may be obtained.

Reference point

Reference point

Membrane
Select the surface element type

Assign references graphically

Assign a reference for the local x axis Assign a reference for the local z axis

User’s Manual

139

Membrane elements may be used to model flat structures whose behavior is dominated by in-plane membrane effects. Membrane elements incorporate in-plane (membrane) behavior only (they include no bending behavior).

F

The element can be loaded only in its plane. AxisVM uses an eight node Serendipity, plane stress (σzz = σxz = σyz = 0, εxz = εyz = 0, εzz ≠ 0) or plane strain (εzz = εxz = εyz = 0, σxz = σyz = 0, σzz ≠ 0), finite element as membrane element. The membrane internal forces are: nx, ny, and nxy. In addition the principal internal forces n1, n2 and the angle αn are calculated. The variation of internal forces within an element can be regarded as linear. The following parameters should be specified: 1. Plane strain or plane stress 2. Material 3. Thickness 4. Reference (point/vector/axis/plane) for local x axis 5. Reference (point/vector) for local z axis Allows browsing of the material library to assign a material to the element. The material selected will be added to the material table of the model. Automatic reference: The axis of element local directions x and z can be determined by reference elements (see… part 4.9.17 References) or can be set automatically.

$
Plate

The center of the membrane elements is displayed on the screen in blue.

Plate elements may be used to model flat structures whose behavior is dominated by flexural effects. AxisVM uses an eight/nine node Heterosis finite element as plate element, that is based on Mindlin-Reissner plate theory that allows for transverse shear deformation effects). This element is suitable for modeling thin and thick plates as well. Plate elements incorporate flexural (plate) behavior only (they include no in-plane behavior).

F

The element can only be loaded perpendicular to its plane. The plate internal forces are: mx, my, mxy moments, and vx, vy shear forces (normal to the plane of the element). In addition, the principal internal forces: m1, m2 , the angle αm and the resultant shear force qR are ca lculated. The variation of internal forces within an element can be regarded as linear. The following parameters should be specified: 1. Material 2. Thickness 3. Reference (point/vector/axis/plane) for local x axis 4. Reference (point/vector) for local z axis

140

AxisVM 8+Release 4

Allows browsing of the material library to assign a material to the element. The material selected will be added to the material table of the model. Automatic reference: The axis of element local directions x and z can be determined by reference elements (see… part 4.9.17 References) or can be set automatically.

$
Shell

The center of the plate elements is displayed on the screen in red.

Shell elements may be used to model structures with behavior that is dependent upon both in-plane (membrane) and flexural (plate) effects. The shell element consists of a superimposed membrane and plate element. The element is flat, so the membrane and plate effects are independent (first order analysis).

F

The element can be loaded in its plane and perpendicular to its plane. The shell internal forces are: nx, ny, and nxy forces (membrane components), mx, my, and mxy moments, and vx, vy shear forces (plate components). In addition, the principal internal forces and moments n1, n2 , the angle αn , m1, m2 , the angle αm and the resultant shear force vSz are calculated. The variation of internal forces within an element can be regarded as linear. The following parameters should be specified: 1. Material 2. Thickness 3. Reference (point/vector/axis/plane) for local x axis 4. Reference (point/vector) for local z axis Allows browsing of the material library to assign a material to the element. The material selected will be added to the material table of the model. Automatic reference: The axis of element local directions x and z can be determined by reference elements (see… part 4.9.17 References) or can be set automatically.

$
Modifying

The center of the shell elements is displayed on the screen in green. Selecting elements of the same type Modifying will be activated. Checked properties can be changed or picked up from another element. Selecting elements of different types Definiton will be activated. See... Pick Up at line elements (4.9.6).

Pick Up>>

User’s Manual

141

4.9.8.

Nodal Support
Nodal support elements may be used to model the point support conditions of a structure. Nodal support elements elastically support nodes, while the internal forces are the support reactions. Midside nodes of surface edges cannot be supported. References are used to arbitrarily orient the x and z axes of the element.The x axis is directed from a reference point to the attachment node (the node to which it is attached). You can specify the translational and/or rotational (torsional) stiffness values about the element axes.

F $

The default stiffness values are 1.000E+10 [kN/m], [kNm/rad]. The support elements are displayed on the screen in yellow (translational spring) or orange (rotational spring). The support can be oriented in a direction: - Global - Reference - Beam/rib relative - Edge relative

You can define only one global support for a node. You cannot define nodal support for a midside node of a surface element. Defines nodal support elements in the direction of a reference (point or vector). You must select the nodes that are identically supported, and specify the corresponding stiffness (translational Rx, and rotational R xx). The direction of the reference vector is defined by the element node and its reference point or reference vector in the following way:

R yy. Buckling) the initial stiffnesses are taken into account.
F $
. R Z) and orange (R XX. R zz stifnesses. tension only (very small stiffness in compression). You must select the beam / rib elements and the nodes that are identically supported. R z and rotational Rxx. R YY. If more than two surfaces are connected to the edge and you select one or two of them then support local system will be determined based on the selected surfaces. Nodal supports appear as brown (R X.142
Reference point
AxisVM 8+Release 4
Reference vector
Support elements oriented toward a reference point Beam/rib relative Defines nodal support elements about local coordinate axes of beam / rib elements. R zz stifnesses. The non linear parameters are taken into account only in a nonlinear analysis. The y-axis is determined according to the right hand-rule. In any other case in the analysis (Linear static. R ZZ) pegs in 3 orthogonal direction. Vibration I/II. R z and rotational Rxx. If one surface is connected to the edge the local coordinate axes of the edge are: x = the axis of the edge y = the axis is oriented toward inside of the surface element in its plane z = parallel with the z local axis of the surface element If two surfaces are connected to the edge the local z-axis direction is bisecting the angle of surfaces. R yy.
Nonlinear behavior
Nonlinear force-displacement characteristics can be specified for this element as follows: compression only (very small stiffness in tension). A resistance value can be also be entered. R y. You must select the surface elements and the nodes that are identically supported. R Y. R y. and specify the corresponding translational Rx. and specify the corresponding translational Rx.
Support elements parallel with a reference vector
Reference point
Edge relative
Defines nodal support elements about local coordinate axes of surface element edges.

. and geometry of the column. Selecting elements of different types Definiton will be activated.9. Calculating nodal support stiffness a column below and a column above the node can be specified separately. Modifying Selecting elements of the same type Modifying will be activated. The columns and walls modeling the supports also appear in rendered view and the cursor can identify them.9. or surface edges. Pick Up at line elements (4.6). Checked properties can be changed or picked up from another element. The support stiffnesses are determined based on the end releases.
. material. These column parameters can also be used in punching analysis (especially in the case of intermediate slabs). while the internal forces are the support reactions. Line support elements (Winkler type) are elastically supporting beams.9. You can specify the translational and/or rotational (torsional) stiffness values about the element axes... button to calculate the support stiffness (including the rotational stiffness) due to a column type support.User’s Manual
143 Load from material library Use the cross-section editor fixed/pinned at the top of column
Support stiffness calculation
Load from the cross-section library Fixed/pinned at the bottom of the column
Use the Calculate.
Pick Up>>
4.. See. ribs.
Line Support
Line support elements may be used to model the line support conditions of a structure.

Defines line support elements for beam/rib elements in their local coordinate system acting as an elastic foundation. R zz) lines in 3 orthogonal direction. R zz stifnesses. The beams/ribs with line supports must be divided into at least four elements.
F $
. The non linear parameters are taken into account only in a nonlinear analysis. kz  
F
AxisVM warns you if the condition is not satisfied (by one or more elements).  2 ky 
4
4 Ex I y   . Vibration I/II. R Z) and rotational (RXX. R yy.
Reference point
Nonlinear behavior
Nonlinear force-displacement characteristics can be specified for this element as follows: compression only (very small stiffness in tension). Buckling) the initial stiffnesses are taken into account. R y. R y. R yy. Line supports appear as brown (Rx. A resistance value can aslo be entered. therefore you can divide the elements and repeat the definition/modification process. You must specify the corresponding translational Rx. R Y. R YY. or [kNm/rad/m]. R z and rotational R xx. You must specify the corresponding stiffness (translational Rx. R y. Defines line support elements parallel to global coordinate axes. If you specify line supports the internal forces are linearly interpolated between the ends of the element.144
AxisVM 8+Release 4
The line support behaves identically in tension and compression and is considered constant within the element. where L is the beam / rib length. therefore the division of the elements is required. R z and rotational Rxx. R yy. R z) and orange (R xx. You must specify the corresponding translational (RX. In this case the Winkler’s modulus of the defined elements are set to zero. In addition.000E+07 [kN/m/m].
Edge relative
Defines edge support elements relative to local coordinate axes of the edges. The line support can be oriented in a direction: Global Beam/rib relative Edge relative
F
Global
The default stiffness values are 1. R ZZ ) stiffnesses. If more than two surfaces are connected to the edge and you select one or two of them then support local system will be determined based on the selected surfaces. tension only (very small stiffness in compression). If one surface is connected to the edge the local coordinate axes of the edge are: x = the axis of the edge y = the axis is oriented toward inside of the surface element in its plane z = parallel with the z local axis of the surface element If two surfaces are connected to the edge the local z-axis direction is bisecting the angle of surfaces. the following condition must be satisfied:
Beam/Rib relative
F
L ≤ lk =
 4E I 1 x z min  4 . In any other case in the analysis (Linear static. R zz). The y-axis is determined according to the right hand-rule.

User’s Manual

145

Support stiffness calculation

Use the Calculate... button to calculate the global or edge-relative line support stiffness (including the rotational stiffness) due to a wall type support. The support stiffnesses are determined based on the end releases, material, and geometry of the wall.

4.9.10. Surface Support

Surface support

Defines a surface support element (Winkler type elastic foundation) to surface elements. You must specify a translational stiffness in the surface element local coordinate system. The surface support behaves identically in tension and compression and is considered constant within the element. You must specify the support stiffness Rx, R y, R z (Winkler’s modulus) about the surface element local x, y, and z axes.

F
Nonlinear behavior

The default stiffness values are 1.000E+04 [kN/m/m], or [kNm/rad/m]. Nonlinear force-displacement characteristics can be specified for this element as follows: compression only (very small stiffness in tension), tension only (very small stiffness in compression), or with resistance (the same stiffness for compression and tension). The non linear parameters are taken into account only in a nonlinear analysis. In any other case in the analysis (Linear static, Vibration I/II, Buckling) the initial stiffnesses are taken into account. Surface supports appear as an orange square-hatched fill.

F

$

146

AxisVM 8+Release 4

4.9.11. Edge hinge
Edge hinge can be defined between domain edges or between a rib and a domain edge. Select edge and a domain. Hinge stifness can be defined in the local system of the edge of the selected domain.

4.9.12. Rigid elements
Rigid elements may be used to model parts with a rigid behavior relative to other parts of the structure. Rigid elements may be used only in a linear static analysis. The elements can be defined by selecting the lines that connect its nodes. The selected lines that have common nodes define the same rigid element. There is no limit to the number of nodes of any element.

Lets you define rigid elements. You must select the lines that connect the nodes attached to rigid elements. Recall that the lines with common nodes define the same rigid element.

rigid

1

2

3

rigid

1

2

You can join or split rigid elements using the modify command. If you select lines that connect nodes of different rigid elements, the elements will be joined. If you deselect lines of rigid elements interrupting their continuity, the respective elements will be split.

F

A finite element cannot have all of its lines assigned to the same rigid body. If we want to calculate the mass of the body in a vibration analysis, place a node to the center of gravity, connect it to the body and make this line a part of the rigid body. Assign the mass of the body to this node. The rigid elements are displayed on the screen with thick black lines.

$

User’s Manual

147

4.9.13. Spring

Spring element

The spring element connects two nodes of the model. The element has its own coordinate system. You can specify the translational and/or rotational (torsional) stiffness values about the element axes. The element can have nonlinear elastic stiffness properties. The element local system can be oriented in a direction: Global Geometry Reference Element relative Node relative

Define

You must select the nodes that are connected, and specify the corresponding stiffness (translational KX, K Y, K Z and rotational K XX, K YY, K ZZ). If a nonlinear elastic spring is to be defined, you can specify resistance values, for each internal force component.

F

Resistances will be taken into account only in a nonlinear static analysis, otherwise they will be ignored. The nonlinear parameters are taken into account only in a nonlinear analysis. In any other case in the analysis (Linear static, Vibration I/II, Buckling) the initial stiffnesses are taken into account (that stay constant during the analysis).

148

AxisVM 8+Release 4

4.9.14. Gap

Gap element

The gap element is used to model point-to-point contact. The element has two states: one active, when it has a large stiffness value (simulates that a contact is achieved); and one inactive, when it has a small stiffness value (simulates that no contact is achieved). This contact model is approximate. The gap element can be active in tension or compression. Typical forcedisplacement diagrams of gaps active in tension and compression are shown below correspondingly.

The gap element is a nonlinear element that can impose difficulties to the solution of the nonlinear problem, due to large changes of element stiffness when it changes status (active/inactive). If the element is used to model regular contact problems, you may allow the element to auto adjust its stiffness, in order to smooth the large stiffness variations (at status changes) that can cause even divergence of the iterative solution process. You must specify with two nodes: Defining local x orientation is the same as for beam elements. Active: The active state that can be tension (a tension bolt connection) or compression (contact of two plates) Orientation (from one of its node to its other node) Active stiffness: By default it is 1E+8 kN/m. Inactive stiffness: By default it is 1E-2 kN/m. Initial opening\penetration: By default it is 0. The initial opening can be set based on element geometry as well (Check By Geometry). The initial opening is a positive or zero value. While the initial opening does not close, the gap is considered inactive.

User’s Manual

149

Auto active stiffness adjustment: If no adjustment is selected, the values below are not taken into account. Minimum allowed penetration: You can set a minimum value for the penetration of the contact condition that is allowed. By default is 1E-05. Maximum allowed penetration: You can set a maximum value for the penetration of the contact condition that is allowed. By default is 1E-05. Maximum adjustment ratio: If the penetration is below the minimum, the active stiffness is softened by a maximum ratio entered here. If the penetration is between the two limits, no action is taken. If the penetration exceeds the allowed maximum, the active stiffness is hardened by a maximum ratio entered here. The default value is 100. In this case, the value of the adjustment ratio is the taken as: 1/100, 1/10, 1, 10, or 100.

F

If the gap element is used in an analysis different from a nonlinear static analysis, the element will be taken into account as a spring with a stiffness corresponding to its initial opening. If the initial opening is zero, the active stiffness will be taken into account.

4.9.15. Link

Link elements

Link elements connect two nodes (N-N) or two lines (L-L) and have six stiffness components (defined in their coordinate system) that are concetrated on an interface (located between the connected nodes/lines). Its position can be entered relative to one node/line that is considered as reference. Link elements can have a nonlinear parameter called limit resistance that limits the force they are able to transfer. Node-to-Node (N-N) Link Connects two nodes. The stiffness components are defined in the global coordinate system. Assigning zero value to a component the corresponding force or moment will not be transferred from one node to the other. The position of the interface can vary from 0 to 1 relative to the master node (selected by the user). If the location of the interface is = 0 the interface is at the master node. If it is = 1 the interface is at the opposite node. For any value greater than 0 or lower than 1 the reference is between the nodes.

150

AxisVM 8+Release 4

Typical applications are: main girder-purlin connection; some types of grillage connections; St. Andrew bracing connections; etc. Example: A main girder-purlin connection (see SteelFrame.axs in the examples folder). Let assume that the vertical axis is Z being parallel to the local z axis. The main girder is an IPE-400 in X-Z plane, the purlin is an I-200. You would like to transfer forces from the purlin to the main girder but not the moments.

These elements are represented by their line of gravity. The link has to be placed between these two axes at their point of intersection (if seen from above). Therefore, this link has to be assigned to a vertical line having a length equal to the distance of axes i.e. 30 cm (40/2 + 20/2). Select the node on the main girder to be the master node of the link. The inter-face always has to be placed at the actual point of contact. In this case the interface is located 20 cm far (40/2) from the master node (i.e. the main girder axis). So the interface position is 20/30 = 0.666. You assume that the connection is fixed against displacements but can rotate. Therefore, you enter 1E10 for translational stiffnesses and 0 for rotational ones. If the purlins are supported only by these links you have to enter KYY=0.001 or a similar small value to eliminate rotation around the main girder axis. Nonlinear parameters A limit resistance can be specified for each corresponding component with non-zero stiffness. Line-to-Line Link Connects two lines with three nodes each that can be rib elements and/or edges of surface elements. A line-toline link has 6 nodes. The stiffness components are defined in the local coordinate system of the link that is in the plane of the link element with the x local axis parallel to the master line, and the local z axis oriented toward the other line in the plane of the link and is orthogonal to the local x axis. Assigning zero value to a component the corresponding force or moment will not be transferred from one node to the other. The position of the interface can vary from 0 to 1 relative to the master line (selected by the user). If the location of the interface is 0, the interface is at the master line (at the start point of the arrow). If it is 1 the interface is at opposite line (at the end point of the arrow). For any value greater than 0 or lower than 1 the interface is between the lines.

. Example: A floor-wall hinged connection. the floor is parallel to the X-Y plane and walls are represented by shell elements.1. Therefore. Let’s assume that the vertical axis is Z. and set the interface location. Link elements are divided according to the domain mesh. Now you can mesh the domains. 3.2 Mesh generation on domain).9.
2. semi-composite / fullcomposite layered beams. The link element(s) are created. Therefore enter 0 for the interface position.3 Domain) and connect the corresponding opposite nodes of the domains with lines (the number of nodes on the edges of the domains should be equal). Elements are represented by their middle plane. the wall is in Y-Z plane. etc..User’s Manual
151
Typical applications are: floor-wall hinged connections. Nonlinear parameters A limit resistance can be specified for each corresponding component with non-zero stiffness. Click OK on the Selection Toolbar. Define the domains (See.5 cm (15/2). (See. When used in conjunction with domains the following steps can be followed to define line-to-line link elements: 1. You would like to transfer forces from the floor to the wall but not the moments.11.
. 4. The distance between the edges is 7. Links have to be placed between the upper wall edge and the floor edge. The wall has to reach until the bottom plane of the floor. The interface has to be at the actual point of contact which is in the bottom plane of the floor and is 0 cm far from the master node. Floor thickness is 15 cm. Click OK on the Selection Toolbar.
5. 4. You assume that the connection is fixed against displacements but can rotate. you enter 1E10 for translational stiffnesses and 0 for rotational ones.. By default the interface is in the midpoint of the link element. 4. Semi-rigid rib-shell connections. In this case the link elements have to be in the plane of the wall. 6. Select wall edge nodes to be the master nodes. Select the quadrilateral between the domains.. Define the link stiffness. Select the master line of the link element.

By setting a digit to c (constrained) the corresponding degree of freedom component is constrained.16. θZ constr. The nodes with DOF different from [f f f f f f] are displayed on the screen in cyan. Overwrite The new setting overwrites the existing degrees of freedom settings of the selected nodes. θX. e Z. In the calculations. Example of union initial code: new code: resulting code: eX free free free eY constr. Union Performs a union set operation with the set of the new degrees of freedom codes and the set of existing degrees of freedom codes of the selected nodes. In the default setting no nodes have constrained degrees of freedom. 1 eX 2 eY 3 eZ free rotation about the specified axis. eZ free free free θX constr. e Z. θY and θZ) are set by a six digit code comprised of f (free) and c (constrained) symbols. you can quickly apply a predefined setting by selecting it from the list box. e Y. in many cases typical combinations of degrees of freedom can be used. Changes will be applied only to those nodal DOF which have their corresponding check-box checked. constr. constr. Notations: free translation.
The six nodal degrees of freedom (eX. By default the nodes are considered free (all digits are f-free symbols). constr.9. e Y and eZ .
F $
The loads that apply in the direction of a constrained degree of freedom are not taken into account. However. You have two options to change nodal DOF. θY and θZ) can be selected.152
AxisVM 8+Release 4
4. The following particular structures are listed: Plane truss girder / Space truss / Plane frame/ Grillage / Membrane / Plate Define a nodal DOF Use the buttons to set the degrees of freedom. free constr. 4 θX 5 θY 6 θZ
. e Y. constr. θY free constr. Each digit corresponds to one degree of freedom component. In these situations.(translations) eX. θY and θZ. θX.(rotations) θX. equilibrium equations will only be written in the direction of the free displacements (translations/rotations). Unchecked components will retain their original values in the selection. Nodal DOF (Degrees of Freedom)
Lets you constrain the six nodal degrees of freedom that are: . Any combination of the six nodal degrees of freedom (eX. This option is useful in the definition of symmetry conditions. constr. Button captions will reflect the current value. The default DOF code of a node is [f f f f f f]. Loads in the direction of the constrained degrees of freedom will appear in the table of unbalanced loads.

z = green. mx. my. Automatic references for rib elements: If the rib is independent the reference vector will be generated and assigned to the element as for the beam elements. the generation of the reference vector is as follows: The reference vector will be parallel to the bisector of the local z axes (normal to the surfaces) of the surfaces that have the rib element attached. In any other case. The element properties are defined and the internal forces (Nx. vectors or axes. References
Lets you define reference points. The reference points are displayed on the screen as small red + symbols. The references determine the orientation of the local coordinate systems of the finite elements in the 3D space. and axes are normalized with respect to 1. and spring elements or to define the positive local x and z axes of surface elements. the reference plane by three points. Vy. mxy for plates. Quick modify: Clicking on the symbol of a reference the Table Browser is invoked displaying the table of the references.154
AxisVM 8+Release 4
4.
$
Reference point
$
. If the rib is connected to a surface element. Tx.) are computed in that local system. The reference points are defined (by its coordinates) in the global coordinate system. and planes. Local z-axis reference If the plane of the surface element is parallel to the Z axis. The following references can be used: Automatic references Automatic references for truss and beam elements: A reference vector is generated and assigned to the truss and beam elements as follows: If the axis of the element is parallel with the global Z axis the reference vector will be parallel to the global X axis. n y. In any other case it will be parallel with the global Z axis. Automatic references for domains and surface elements: Reference vectors will be generated and assigned to the surfaces as follows: Local x-axis reference If the plane of the surface is parallel with the X-Y plane the reference vector for the x local axis will be generated as a vector parallel with the global X axis. nx. In any other case it will be parallel with the global Z axis. the generated reference will be a vector oriented toward the origin of the global XYZ system. Mz for beams. n xy for membranes. support.17. Color codes: x = red. etc. The reference vector and axis can be defined by two points. y = yellow. rib. The local coordinate system of the elements defined with the references is used to define cross-sectional properties and to interpret results. it will be parallel with the intersection line of the surfaces and X-Y plane. My. Vz.9. Reference point is used to define the orientation (local coordinate system) of beam. When closing the table the reference vectors.

Reference point
Supports: In the case of a support element you can use a reference point to define local x axis.
Reference point Reference point
Surface elements: The positive local z axis is oriented toward the half-space in which the reference point is located. The positive local y and z axis direction is determined by the right-hand rule. The reference vectors are displayed on the screen as red arrows. In the case of a surface element the reference point must be located in the plane of the element. support. and springs: The reference point and the element’s local x axis defines the local x-z plane.User’s Manual
155
Beams. ribs. and is perpendicular to the element’s plane. Also defines the orientation of local z coordinate axis of beam. Once the local x-axis is defined local y-axis is determined according to the right hand-rule. and spring elements.
Reference point Reference point
The local x axis will be oriented in the direction of the reference point.
Reference point
Reference vector
Lets you define the local x axis for surface. rib and spring elements.
$
.

ribs. The reference axis must not include element centerpoint. The positive local y and z axis direction is determined by the right-hand rule. The orientation of local z-axis can also be defined by a reference vector. In the case of a surface element the reference vector must be parallel with the plane of the element.156
AxisVM 8+Release 4
Surfaces: The local x axis will be parallel with the reference vector.
Supports: In the case of a support element you can use a reference vector to define local x axis.
Reference vector Reference vector
Reference Axis
Reference axis is used to define the local x-axis of surface elements.
Beams.
. and springs: The reference vector and the element’s local x axis defines the local x-z plane.
$
The reference axises are displayed on the screen as red arrows. that will be oriented towards the reference axis.

F
Deleting an architectural object having a static model will not delete its associated static model. that will be parallel to the intersection line of the reference plane and the plane of the element.
Display
Select architectural project stories and element types you want to be displayed. The reference plane is displayed on the screen as a red triangle.) as a background layer.ACH) or an IFC file (*.
Reference angle
Rotation of truss / beam / rib cross-sections is made easy by the reference angle. 3. In any other case the angle is relative to the global Z axis.
.
F
Delete Objects
Click this button to delete selected architectural model objects. Click the Property Filter icon to select beams and columns within a certain range of section size according to their minimum side length or select walls or slabs within a certain range of thickness. If you want to restore the whole range click the button at left bottom.6 Import. If the Only objects without static model is checked only elements not having static model will be selected. the angle is relative to the global X axis. If you create model framework or delete objects and nothing is selected the Selection Toolbar appears.User’s Manual
157
Reference Plane
Reference plane is used to define the local x axis of surface elements.. Creating model framework from an architectural model
This icon starts the conversion operation of the architectural model if previously an ArchiCAD interface file (*. The automatic local coordinate system (and the cross-section) can be rotated around the element axis by a custom angle. The reference plane must not be parallel with the plane of the element.
$
4. Use the built-in Filter to enhance selection. If the element is parallel with the global Z direction.18.9..IFC) was loaded by File / Import (See.1.

Parts will automatically be created for levels and object types and the elements created for the static model will be included in the appropriate parts. Framework nodes and lines become part of the AxisVM model and are independent of the background layer.
. Columns will be reduced to their axis. Assign a material and a thickness. For layered walls you can choose to apply the thickness of the load bearing layer. the total thickness or a custom value. walls. The support stiffness will be computed based on the top and bottom end releases. You can assign properties to the selected architectural objects as follows: Slab Floors can be defined as plates or shells. For layered floors. Apply bottom support: You can automatically assign a support to the bottom edge of the selected walls. the thickness of the layers will appear in the layer list.
Convert walls to supports: You can convert wall objects to supports by enabling this checkbox. You can select the layers that you want to take into account.
Load from Material Library
Wall
Walls can be defined as membranes or shells. The support will be placed at the top edge of the corresponding wall.158
AxisVM 8+Release 4
Create Model Framework
Model framework will be created from selected layer elements. Hinged wall connections can be modeled using edge hinges when creating a model framework from the architectural model. Assign a material and a thickness. slabs and roofs will be reduced to their center plane.

Assign a material and a crosssection. the thickness of layers will appear in the layer list. The support stiffness is established based on the end releases.User’s Manual
159
Column
Graphical Cross Section Editor Cross-section Library
Column objects are always converted to beam elements.
.
Roof
Roof objects are always converted to shell elements. If Auto is selected the cross-section is created based on the geometrical description of the architectural object. Beam Beam objects are always converted to beam elements.
Convert columns to supports: The selected column objects can be converted to supports. You can assign a support to the bottom of the column. The supports will be placed at the top of the column. For layered roofs. If Auto is selected the crosssection is created based on the geometrical description of the architectural object. Assign a material and the cross-section. You can select the layers that you want to take into account. Assign a material and a crosssection.

Click the OK button to apply the modifications and exit the dialog window. 5. 2. 3. Property fields show the common value in selection. lines or surfaces.
.5 Delete
4.. If more finite elements have been selected they can be immediately modified by clicking one of them.20.
F
In fact.9. If you click an element which is not selected.
4. If you click on a node its nodal degrees of freedom can be edited immediately. 3. Modify
Lets you modify the definition of the selected elements. If selected elements have different values the field is empty.9. In the element’s dialog window check the properties you want to modify. 3. but does not assign properties to undefined geometrical elements and allows access to a specific property without altering others. Loads
Lets you apply various static loads for static and buckling analysis.2. selection disappears and you can modify the element you clicked.160
AxisVM 8+Release 4
4.19.5. the modification is similar to the element definition. Modify the respective properties as desired.. Delete
[Del] See. You can also modify the properties using of Property Editor. Holding the [Shift] key down. Click the element’s icon on the Elements Toolbar.. select the elements to modify. If the Geometry or Elements tab is active click a finite element to modify its properties. 1. See. and define concentrated masses for vibration analysis. You can use the Selection icon as well. You can switch to the element definition radio button to define all properties of all the selected elements.1 Property Editor
Immediate mode
4..10.

User’s Manual
161
4. Influence line Lets you apply a relative displacement load to obtain the influence line of a result component. and buckling analysis. Load groups can also be created from the different load cases. Load Cases. create new. the loads can also be taken into account as masses. Static The static load case can be applied to static. Any load you create will be stored in the current load case. Load groups can also be created from the different load cases. You must assign a different name to each case. vibration.
Load Case
New Case
Lets you set the current. and modify or delete existing load cases. create new. When calculating the critical load combination. In the professional version the number of load cases is not limited. the load case will be taken into account according to the parameters of the load group to which it belongs.
F
When the influence line load case type is selected you can apply only the influence line load ->
. 2. The load case can be included into a load group. of a truss or beam element.10.1. The following are the three types of load cases that you can choose from when you want to create a new case: 1. In the professional version the number of load cases is not limited. In the standard version a maximum of 99 cases can be created. and modify or delete existing load cases. Load Groups
Load Case Lets you set the current. In the standard version a maximum of 99 cases can be created.
F
Critical combination can be determined only from the results of a linear static analysis. In case of vibration analysis. Any load you create will be stored in the current load case.

name-TI will contain long term values of the equivalent load. that contain the critical combinations. so the Tensioning Dialog will appear. AxisVM generates seismic loads case. After defining a load case with the name name. See. After definition just loads for name-T0 will be calculated as static analysis results are required to determine the long term equivalent loads. and a factor that will multiply the loads while copying.
Duplicate
F
Delete
F
The name of the selected load case will appear in the Info window and the loads you define will get to this load case.
Display order of load cases can be set by the following options. and -. Based on the mode shapes.. Sort by alphabetical order Sort by load groups Follow creation order
. Move up selected case. The two additional cases corresponds to the signs +.. 4. Lets you delete the selected load case. You must specify the new name. select Order of load cases to get to a dialog setting the load case order. where k is the number of available smallest frequencies. Tensioning If tensioning calculation according to the current design code is supported.162
AxisVM 8+Release 4
3. Move selected case to the end.10.21 Tensioning Lets you make a copy of the selected load case under another name. Move down selected case. In case of choosing Tensioning load case only the Tensioning Icon will be active on the toolbar. See. See details… 4. Move selected case to the top. Selected loads can be copied or moved to another load case by changing load case during the copy or move process. These load cases always get into a tensioning load group. and on the structural masses. 4.
Order of load cases. Any of these load cases can be selected to define tensioning. name-T0 will contain the equivalent load calculated for the end of tensioning process. tensioning load cases can be created. two load cases will be created.. you must perform a vibration analysis. This dialog is also available in the Table Browser (Format / Order of load cases).10.10..21 Tensioning Click right mouse button over the list... You can change the current load current case by selecting from the drop down list near the load case icon. The factor can be a negative number as well. in a k+2 number. Click on it then select the proper beam or rib elements.20 Seismic Loads
F
In case of selecting seismic load case only the Seismic parameters icon will be available -> 4. Prior to creating an seismic load case. Seismic When selecting seismic load case type you can specify the parameters for calculation of earthquake loads.

Load groups are used when generating of critical (design) values of the results. Clicking any icon within the New Group group box will create a new group in the tree and you can specify a name for it. 2.User’s Manual
163
Load group
You can select the load group you want to place the current load case in from the dropdown list. Changing the safety class may require changes in the incidental group factors γf. and the corresponding factors according to the current design code..
Safety Class Load Group New Group
Select the safety class of the building from the combo box. Only one load case from the group will be taken into account in a load combination at one time. dynamic factor.10. Exceptional Includes earthquake. Incidental Includes live load. Include all load cases in combinations All load cases from the group will be taken into account in all load combinations with their upper or lower safety factor. After creating a load group you have to specify the value of its paremeters (like the safety factor.. incidental. 3. snow load.).2 Load Combination The following load groups are allowed depending on the design code: 1..q. etc. permanent features on the structure. Ψ and Ψt. Setting the current load case : Click on any existing load cases from the list which is on the left side of the Load Groups & Load Cases dialog window.. exceptional) of the load group. See. simultaneity factor. 4.. You can also drag and drop load cases between load groups by mouse.. Mutually exclusive load cases In a critical load combination only one load case from the group will be taken into account at one time.. Any subsequently defined loads will belong to the newly selected load case. You must specify the name and the type (permanent. Load case will immediately be moved to its new position in the tree view. explosion. Can be simultaneous with exceptional goups If checked load case(s) from the group can act together with a load case from an exceptional group in critical combinations. support settlements. That load case must have the simultaneity factor of α = 0 . collision. Lets you define a new load group. Simultaneous load cases Any number of load cases from the group can act simultaneously in critical combinations. Permanent Includes dead load. Include the most unfavourable load case only Only the most unfavourable load case will be taken into account from the load group with its upper or lower safety factor. crane runway load. A load case can be assigned to a load group by choosing a group from the dropdown list or dragging the load case under a load group in the tree. Later you can specify which load cases belong to a specific load group. Existing load group names will be rejected. wind load..
. The chosen load case will become the current case.

membrane. It can contain only tensioning load cases. That load case must have the simultaneity factor of α = 0 . In case of nonlinear static analysis. plate. shell truss. shell truss.rib
4. Seismic load group (Eurocode.164
AxisVM 8+Release 4
4.
F
You can also define load combinations after you have completed a linear static analysis. Inserts a load combination table to the current report. membrane.2. Load types The following loads can be applied to the elements: Load Concentrated Line (distributed) Edge (distributed) Dead load Temperature Fault in length Tension/Compression Forced support displacement Fluid Seismic Influence line Tensioning Element node. and then performs the analysis (a load combination at a time). Tensioning load group (if tensioning can be calculated according to the
current design code) Tensioning load group is handled as a permanent load group. STAS and Italian code) Only one load case from the group will be taken into account in a load combination at one time. rib. Both load cases for the same tensioning (name-T0 and name-TI) cannot be included in any load combination. shell plate. beam beam. rib. membrane.
5. plate. shell node truss. DIN 1045-1. beam truss. beam. membrane. Then. beam. Load Combination
Lets you define load combinations of the defined load cases. Calculates all critical combinations based on load groups and transfers them into the load combination table. when required the postprocessor computes the results of these load combinations. shell truss. The results of a load combination will be computed as a linear combination of the load cases taking into account the specified load case factors. A zero factor means that the respective load case does not participate in the load combination. beam support plate. beam beam. AxisVM first generates the combination case.10. You can specify a factor for each load case in a load combination. plate.
. rib. SIA 26x.

in the global coordinate system. You must specify the values of the load components FX. Move them to their new position. Select the loads you want to move together. Grab any of them by pressing the left mouse button. F Y. 3. 2. (Enter or Space). MY. FZ and MX.166
AxisVM 8+Release 4
4. Modify nodal loads Modify position You can select. the moments as green double arrows. 4. Signs of the load values are calculated according to the right hand rule. a rib or a domain.
Modify value
F $
. copy or modify the load independently of the node. The forces are displayed on the screen as yellow arrows. 1. move. If you apply a nodal load to a node that is already loaded. Click the Nodal Load icon on the Toolbar.10. Select the load. Click the left mouse button or use a command button. 1. you can overwrite or add it to the existing load. MZ. Change the values Nodal loads can be moved onto a beam. Load components applied in the direction of a constrained degree of freedom will be not taken into account in the analysis. The positive directions are according to the positive directions of global coordinate axes.3. Nodal Loads
Lets you apply forces/moments to the selected nodes. 3. 2.

Reference (with respect to a reference)
.
4.Global (with respect to the global coordinate system) . See. You must specify the values of the load components FX. You can place loads by clicking the left mouse button or pressing any of the command buttons. Concentrated Load on Beam
Lets you apply concentrated forces/moments to the selected beam finite elements.User’s Manual
167
4. 4.4. The positive directions are in accord with the positive directions of the local or global coordinate axes. F Z..
$
The forces are displayed on the screen as yellow arrows. moved. MY.5. If you apply a concentrated load to a node that is already loaded. You can also enter the location of the load by its coordinates. Modify load values like in case of nodal loads.7.10. MZ in the local or global coordinate system..Local (with respect to the local (element) coordinate system) . you can overwrite or add it to the existing load. F Y. MX. the moments as green double arrows. modified independently of the beam. Point Load on Domain
Applies a point (concentrated) load at the location of the cursor if it is over a domain. copied.2 Entering Coordinates Numerically The direction of the load can be: .10. Concentrated loads can be selected.

Enter the new load values in the dialog. Click on the Modify button to apply the changes and close the window. Keep left mouse button depressed.
. 4. 1. Select the load with the cursor. Move the mouse or enter the relative coordinates to move the load to a new location. Modify load values like in case of nodal loads. 3. copied.
F
Modifying domain mesh leaves the concentrated loads (applied on the domains) unchanged. Modify of a load Line loads can be selected. Click the left mouse button.168
AxisVM 8+Release 4
Modify point load on domain Modify position
You can modify the location and value (intensity) of the load: 1. 3.
Modify value
The load value can also be changed in the Table Browser. Release left mouse button to set the load in its new location. You can apply multiple distributed loads to a beam/rib in the same load case. 2. moved. Distributed line load on beam/rib
Lets you apply constant or linearly distributed forces and torque to the selected beam/rib finite elements. modified independently of the beam or rib.
4. 2.6.10. Select the load with the cursor (a load symbol appears beside the cursor). 4.

the location and the values of the load components in the local or global coordinate system as follows: Loads in local coordinate system Loads in global coordinate system
You have to specify the following parameters: Direction: local or global coordinate system Distribution: along length.7. the value of the load that is applied to the beam/rib is p ⋅ sin α . mTOR2 If the load is projective. Edge Load
. mTOR1 End location: x2 relative to the i-end End value: px2.
F
For rib elements you can apply line loads distributing along the entire length of the rib only. p y1. p y2. p z2. projective Location definition: By Ratio (0 • x 1 < x 2 • 1) or By Length (0 • x 1 < x 2 • L) where L is the length of the beam/rib Starting location: x 1 relative to the i-end Starting value: px1. p z1.
4. where α is the angle of the load direction and the beam/rib axis.10.User’s Manual
169
You must specify the distribution.

If more than two finite elements are connected to the edge or they have different local coordinate systems you have to select both the edge and the finite element when you specify the local load. Element Load in Local Directions (in Local Coordinate System) Load in Global Directions (in Global Coordinate System)
x
-
-
Membrane
y
-
-
Plate
z
-
-
x
X
Shell
y
Y
z
Z
In the case of shell elements.170
AxisVM 8+Release 4
Lets you apply distributed (constant) loads to the selected edges of the selected surface elements. the value of the load that is applied to the shell is p cos α . Load will be defined in the local system of the selected element.
. If the load p is projective. where α is the angle of the load direction and the element plane normal. the load that is applied in global coordinate directions can have a projective distribution.

Enter new load values in the dialogue window.
F
. 2. 3. 4. 4. You can modify the location and value (intensity) and any vertex of the load polyline: 1. 2. The load value can also be changed in the Table Browser. The mx is always the torsional moment (around the application line of the load). Drag the vertex to its new position after pressing the left mouse button. Select the load with the cursor (a load symbol appears beside the cursor). Select the load with the cursor. Deleting the line deletes the load. 4. Set load components and placement method then draw the load (or click the lines) to place it. Click on the Modify button to apply the changes and close the window.8. Keep left mouse button depressed.
Modify of the load Modify location
Modify shape
Modify value
Delete
Select the loads you want to delete and press Delete. Move the mouse or enter the relative coordinates to move the load to a new location.10. 1. Moving the boundary or the internal line moves the load as well. global along element or local. 3. Modifying domain mesh leaves line loads (applied on the domains) unchanged. 1. Release left mouse button to set the load in its new location. Click the left mouse button 3.User’s Manual
171
4. Domain Line Load
Applies a uniform or linear distributed line load over a domain. Click the left mouse button.
Line load between two points
Line load along a polyline
Distributed line load on an existing line or arc
Click any line or arc on the domain boundary or within the domain to apply the load previously defined. Click the left mouse button. The direction of the load can be global projective. This type of load is associative. Move the cursor above the vertex (a load polyline vertex symbol appears beside the cursor). 2.

p z) 2. New distributed domain load definition always overwrites the previous one.User’s Manual
173
4.10. You can select between constant or linear load intensities and set if loads disapper over holes or are distributed on the edge of the hole. Enter load components (px. If you enter the polygon by clicking on the domain close the polygon by clicking on the first vertex again or by double-clicking at the last vertex. For a plate domain the load must be perpendicular to the plane of the domain. Enter three corners of the rectangle by clicking or by coordinates. p y. Steps of load definition in case of constant load: Constant load
Loads disappear/ allowed on holes
Rectangular area load
1. p z) 2. Enter load components (px. Within a load case you can apply only one load of this type on a domain. p y. Enter load components (px.
Polygon load
. Domain Area Load
Applies a mesh-independent area load to a domain. p z) 2. The first icon represents the option that loads over holes are not applied to the structure. Enter load components (px. p y. For a shell domain any load direction is acceptable. Instead of the left mouse button you can also use Space or Enter key to enter polygon vertices. Enter polygon vertices by clicking or by coordinates. Click on the domain Distributed domain load The load will be distributed over the domain. a global projective load or a local load and the components will be interpreted accordingly. 1. The domain element type determines the load type and direction as follows. p y. The shape of this type of load will automatically follow any change in the domain geometry. p z) 2. In this latter case press an extra Enter after specifying the last position. The second one represents the option that loads over holes are distributed on the edge of the hole. Enter two diagonal end points of the rectangle by clicking or by coordinates. (This function is available only on the X-Y. For a membrane domain the load must be in the plane of the domain. The load can be a global load on surface. Y-Z and X-Z planes)
Skewed rectangle area load
1.10. 1.

p 2. Press the left mouse button and move the mouse. Change the load intensity values. 1. Press the left mouse button and move the mouse. If you want to use the same reference points and values to many loads of different shape and position you can lock the reference points and values by clicking the Lock button. Enter polygon vertices by clicking or by coordinates. Enter three reference points by clicking or by coordinates. p 3). 3. In this latter case press an extra Enter after specifying the last position. 4. (3)] in the plane of the domain. shape and intensity of a mesh-independent area load can be changed. Place the vertex by clicking the left mouse button or pressing the Space or Enter key. 1. 1. 3. 1. 2. Enter load values at the reference points (p1. p 3). Enter three corners of the rectangle by clicking or by coordinates. Enter load values at the reference points (p 1. Click the left mouse button. Define load value reference points Lock/unlock value reference points 1. Enter three reference points by clicking or by coordinates. Loads are applied by entering an area. 4.
Modify intensity
. 2. 2. 3. Find the new load position by moving the mouse or by coordinates. Within a load case you can apply only one load of this type on a domain. 2. 3. p 2. 3. p 3). p 2. 1. Click on the Modify button to confirm the changes. Enter two diagonal end points of the rectangle by clicking or by coordinates. New distributed domain load definition always overwrites the previous one. Place the mouse above a vertex of the load polygon (the cursor will identify the load polygon vertex as a corner). Click on the domain. Enter three reference points by clicking or by coordinates. The area load windows appears. Enter load values at the reference points (p1. Instead of the left mouse button you can also use Space or Enter key to enter polygon vertices. Find the new vertex position by moving the mouse or by coordinates. (This function is available only on the X-Y. 3. Place the mouse above the load contour (the cursor will identify the load). 2. p 2. p 3). Enter load values at the reference points (p1.
Rectangle area load
Skewed rectangle area load
Polygon load
Distributed domain load
Modify shape
1. Drop the load by clicking the left mouse button or pressing the Space or Enter key. 2.The load shape will change. Modify area load Modify position The position. These points are the load value reference points. 2.174
AxisVM 8+Release 4
Steps of load definition in case of linear load: Linear load
The plane of the load intensity can be specified by load intensity values (p1. Place the mouse above the load contour (the cursor will identify the load). 4. Y-Z and X-Z planes) 3. If you enter the polygon by clicking on the domain close the polygon by clicking on the first vertex again or by double-clicking at the last vertex. p 3) at three points [(1). p 2. Enter three reference points by clicking or by coordinates. (2).

User’s Manual
175
Multiple loads can be selected and modified this way. 4. Auto distributes the load over the elements under the load. Local directions are defined like automatic references for domains.10. Area load intensity and shape can also be changed in the Table Browser by changing the appropriate values in the load table. Select lines using the selection toolbar. See. The fourth method on the icon tollbar is to click lines of a closed beam/rib polygon. p Y. Distribution remains the same if a new beam or rib is defined under the load.
Load direction can be global on surface.. p Z) The load polygon can be a rectangle. a skewed rectangle or any closed polygon. It is useful when modelling snow or wind load on beam structures. Moving the elements or their end nodes changes the load polygon accordingly.
.
2. (pX. global projective or local. Surface load distributed over beams and ribs
A constant surface load can be distributed over beams and ribs. 1. This way the load becomes associative. Enter load values into the edit fields.17 References. Any new beam or rib defined under the load will redistribute the load.9.
To selected elements only distributes the load over the selected elements only. Click the icon and select the load distribution range in the dialog.
F
4. Define load polygon the same way as for a constant domain area load..11. Delete Select the loads to delete and press [Del] Mesh-independent loads are not affected by removing or re-creating a meshes on domains.

Fault in Length (Fabrication Error)
This load type is used when a structural beam element is shorter or longer than required due to a fault in manufacturing. The load is applied as a distributed load in the direction of the gravitation vector. draw a selection frame around the elements.10. which is required to force the shorter/longer beams to fit the distance of the corresponding nodes. dL [m]. The actual load is calculated from values computed at the corner of the elements.
$
A dashed line is drawn along line elements or surface/domain contours. the mass density of the material. The dead load is computed based on the cross-sectional.e. Fluid loads created with the same definition will be handled as one load. i. A positive dL means that the beam is longer by dL. Dead Load
Lets you take the dead load of the elements (that have materials assigned) and domains into account in the analysis. The load has the same effect as the dT
=
= dL (α ⋅ L) thermal load. Fluid Load
Lets you apply pressure loads characteristic to fluids to the selected plate or shell elements. To change a fluid load only on certain elements use partial selection. to the selected elements. If load intensity labels are turned on a light blue G appears.
4. So if you specified a fluid load on more than one element and click on the load contour on any of these elements the load will be selected on all of them and you can easily change the load parameters. You must specify the value of the manufacturing fault.14.13.
. the gravitational acceleration g.12. Lets you apply the load. and the length or area of the element.176
AxisVM 8+Release 4
4.10.
4.10.

the temperature of the top cord (in the corresponding local direction) T2: .15.
. yG. Thermal Load on Line Elements
Lets you apply temperature loads to the selected (truss. A positive dT means a warm up of the truss. Hz are properties of the cross-section. beam.10.
Beam/Rib
Tref: .reference temperature (corresponding to the initial unstressed state) T1: . You must specify values for the following parameters: Truss
line
elements
Tref -reference temperature (corresponding to the initial unstressed state) T -the temperature assumed for the analysis dT= T . in local y direction: T = T2 + (T1 − T2 )
=
yG Hy zG Hz
in local z direction: T = T2 + (T1 − T2 )
where.16. z G. Tension/Compression
Lets you define an initial axial internal force in truss/beam elements. = A positive dT indicates a temperature increase of the beam. = The load has the same effect as a dT = − P (α ⋅ E ⋅ A ) thermal load.T2 is the non-uniform temperature variation that is taken into account in the analysis. dT#=T1 .the temperature of the bottom cord (in the corresponding local direction) dT =T . where T is the temperature of the cross-section in its center of gravity. and/or rib).User’s Manual
177
4.T ref is the uniform temperature variation that is taken into account in the analysis.
4.Tref is the temperature variation that is taken into account in the analysis. and Hy.10.

You must specify the values of the forced displacement components (translational: e [m].
Reference point
=
T1
T2
F
For membranes only dT is taken into account.
=
4.T2 is the non-uniform temperature variation that is taken into account in the analysis. AxisVM approximates the problem.10. Thermal Load on Surface Elements
Lets you apply temperature loads to the selected surface elements. Forced Support Displacement
Lets you apply forced displacements to the selected support elements. where T is the temperature in the center of gravity of the crosssection. You must specify values for the following parameters: Tref: .17.10. rotational: θ [rad]). by applying a force Psupport in the direction of the support element so as to produce the forced displacement e. dT#=T1 .the temperature of the bottom cord (in the negative local z direction) dT =T . For plates only dT# is taken into account.
.Tref is the uniform temperature variation that is taken into account in the analysis.178
AxisVM 8+Release 4
4.the temperature of the top cord (in the positive local z direction) T2: .18.reference temperature (corresponding to the initial unstressed state) T1: .

Influence Line
Lets you apply a relative displacement load to obtain the influence line of an internal force component.10. See. on the selected truss/beam elements. You must specify the value of the relative displacement e as +1 or -1... Check this assumption every time.
F
Truss
You can define influence line load. If the stiffness of the support element is large enough.19. Load Groups You can specify the value of the relative displacement ex as +1 or -1. A positive forced displacement moves the node in the positive direction of the local axis. by checking the displacement results and verifying the displacement at the respective node.4.10.User’s Manual
179
Psup port = K sup port ⋅ e
where Ksupport is the corresponding support stiffness. only in an influence line type load case. you may apply forced displacements only to the supports stiff enough relative to the stiffness of the structure (at least 10 3 times larger) in the corresponding direction.1 Load Cases.
.
4. Therefore. the secondary deflections due to other loads will be negligible.

In Eurocode 8 the requirement is • • 0. Z directions in the Table Browser.10. Seismic Loads
The seismic loads are taken into account according to the Response Spectrum Analysis method. setting parameters These are the steps of creating seismic loads and setting response spectrum parameters: 1. Y. Based on these vibration mode shapes AxisVM generates equivalent static loads (for each vibration mode shape) which are then applied to the model in a static analysis. This method requires a previously calculated number of undamped free vibration frequencies and the corresponding mode shapes. Seismic load generation.g.20.9 (the sum of the coefficients must represent at least 90% in each direction) and every mode shape having a coefficient larger that 5% in any direction must be included. Vibration results will appear only if you call Table Browser from the Vibration tab page. Check the table of seismic equivalence coefficients in X. Calculate the first n vibration mode shapes and frequencies. Any other supplementary analysis required by the design codes must be completed by the user.180
AxisVM 8+Release 4
Beam
You can specify the value of the relative displacement ex/ey/ez/θx/θy/θz as +1 or -1. AxisVM can calculate extra torsional moments due to random eccentricities of masses and check the sensitivity of stories to second order effects. Then internal force results obtained for each mode shape are summed using to the method described in design code specifications.
.
4.133-81) The program performs only the analysis described below.
Design codes
F
Each design code requires that the mode shapes must represent a certain ratio of the total mass. Seismic analysis can be performed based on the following design codes: • Eurocode 8 (EN 1998-1:2004) • DIN (4149:2005-04) • Swiss code (SIA261:2003) • Romanian code (P 100-92) • Italian code (OPCM 3274) • Hungarian (MI-04. E.

Load cases with endings 4+ and 4-. Create a new seismic load case. The result of these cases will contain the maximum displacements and forces summed up from seismic effects in X. Y or Z direction. The program will create multiple load cases:
a. Setting seismic parameters Clicking this button you can set the response spectrum and other parameters. Ya. Yb. The results of these load cases will contain the maximum forces and displacements calculated from the sum of Xb. The results of these load cases will contain the maximum forces and displacements calculated from the seismic effect in X or Y direction and the torsional effect with a + eccentricity (Xa and Ya) or with a – eccentricity (Xb and Yb).User’s Manual
181
2. Load cases with endings + and –. The results of these load cases will contain the maximum forces and displacements calculated from the sum of Xa. The results of this load case will contain the maximum forces and displacements calculated from the seismic effect in Z direction. Load cases with endings 3+ and 3-. Load cases with endings 1+ and 1-. Yb and Z with a + or – sign. The results of these load cases will contain the maximum forces and displacements calculated from the sum of Xa. Ya and Z with a + or – sign.
F
The effect of seismic forces in Z direction will be taken into account only if a vertical response spectrum is defined. 3. b. Ya and Z with a + or – sign. Load case with ending Z. The results of these cases will contain the positive and negative maximum displacements and forces summed up from seismic effects in X. The results of these load cases will contain the maximum forces and displacements calculated from the sum of Xb. Load cases with endings 2+ and 2-.) With extra torsional effects: Load case with endings Xa. Select any of these cases. Y and Z. Yb and Z with a + or – sign. Xb. Y and Z direction.
.) Without extra torsional effects: Load cases with endings X.

Vtot is the total seismic shear force above and on the story coming from a seismic effect in X or Y direction. h Seismic parameters (Eurocode 8)
Design ground acceleration Behaviour factor for displacements Soil class Spectrum editor Design response spectrum parameters
is the interstory height
Seismic parameters.
On the third tab page you can choose the combination methods. Ptot is the total gravitational load above and on the story dr is the interstory displacement calculated from the differences of average displacements between stories with a seismic effect in X or Y direction. Segment points listed on the left hand side can be edited. response spectra and combination methods can be set in a dialog. Spectral function editor Setting the Design spectrum type combo from Parametric to Custom and clicking on the Spectral Function Editor icon a dialog appears.User’s Manual
185
θ=
Ptot ⋅ dr Vtot ⋅ h
where.
. Spectrum can be created/modified as a function consisting of linear segments.

. response spectra and combination methods can be set in a dialog. Vtot is the total seismic shear force above and on the story coming from a seismic effect in X or Y direction. Segment points listed on the left hand side can be edited. Spectral function editor Setting the Design spectrum type combo from Parametric to Custom and clicking on the Spectral Function Editor icon a dialog appears. h Seismic parameters (SIA 261:2003)
Design ground acceleration
is the interstory height
Importance factor of the building Behaviour factor for displacements Spectrum editor
Soil class
Design response spectrum parameters
Seismic parameters. Spectrum can be created/modified as a function consisting of linear segments.User’s Manual
189
θ=
Ptot ⋅ dr Vtot ⋅ h
where Ptot is the total gravitational load above and on the story dr is the interstory displacement calculated from the differences of average displacements between stories with a seismic effect in X or Y direction.

20. max + j
∑ 0. In other cases the CQC method will be chosen.
4. Combinations of the components of seismic action The quadratic formula or the 30%-method can be chosen.5 ⋅ E
i
2 i
(i ≠ j)
where E is a displacement or force component value at a certain point.
. If Tj / T i < 0. the modal responses can be considered to be independent) then the program choose SRSS method.9 is true for all vibration mode shapes (i.133-81)
Seismic forces are
Sik = Qk ⋅ k g ⋅ k s ⋅ kt ⋅ β i ⋅ Ψ ⋅ ηik
where Qk kg ks kt ˆi • ƒik i k weight of the kth point of mass seismic constant importance factor subsoil and foundation factor dynamic factor damp factor is the mode shape ordinate reduced according to its seismic coefficient mode shape index direction
Combination of modal responses in one direction
E = E 2.User’s Manual
193
Combination methods
Combination of modal responses It is possible to let the program choose the combination method of modal responses by turning on the Automatic radio button.4.e.10. Seismic calculation based on Hungarian Code
Hungarian Code (MI-04.

9 is true for two neighboring modal shape periods the displacement and force values are added ( E j . When creating a seismic load case two different cases will be created with an ending of + and –.194
AxisVM 8+Release 4
F
If T j / Ti • 0. Seismic calculation based on Romanian Code Romanian Code (P 100-92) Seismic forces are
' Skr = ks ⋅ α ⋅ β r ⋅ Ψ ⋅ ηkr ⋅ Gk
where ks ˜ ˆr • ƒ’kr factor depending on the seismic zone importance factor of the building dynamic factor damp factor is the mode shape ordinate reduced according to its seismic coefficient
Gk weight of the kth point of mass k mode shape index r direction
Combination of modal responses in one direction
E=
∑E
i
2 i
where E is a displacement or force component value at a certain point. j +1 = E j + E j +1 ) and used as a separate value in the above formula. These load cases can be used to build combinations and determine critical load combination.
F
The resultant forces are always positive.
.
Seismic parameters (Hungarian Code)
4.5.10. Combination of spatial components Resultant maximum displacement and force values can be calculated from the coexisting effects in X and Y direction:
2 2 E = E X + EY
where EX and EY are the maximum values of independent seismic effects in X and Y direction. in the second case negative. In the first case forces will be positive.20.

F
The resultant forces are always positive.
.User’s Manual
195
F
If T j / Ti • 0. and in general lead to over-dimensioning. When creating a seismic load case two different cases will be created with an ending of + and –.
Seismic parameters (Romanian Code)
where Τc : corner period Ve: velocity of the seismic wave Lc : the biggest horizontal size of the structure A warning message is sent if following inequality is not satisfied:
Lc V e ⋅ Tr
<
1 3
F
If a warning message is displayed. Combination of spatial components Resultant maximum displacement and force values can be calculated from the coexisting effects in X and Y direction:
2 2 E = E X + EY
where EX and EY are the maximum values of independent seismic effects in X and Y direction. in the second case negative. These load cases can be used to build combinations and determine critical load combination.9 is true for two neighboring modal shape periods the displacement and force values are added ( E j . In the first case forces will be positive. j +1 = E j + E j +1 ) and used as a separate value in the above formula. the results of the analysis are inaccurate.

21. Tensioning
Tendons can be assigned to a continuous selection of beam or rib elements. Copied tendons inherit the original parameters and the tensioning process assigned to them. Tendon trajectory tables can be generated with user-defined steps. The first tab is to define tendon parameters and geometry. After completing a static analysis it determines the time dependent losses of prestress and the long term equivalent loads from the result of quasi-permanent combinations (load case name-TI).
.
Prestressing (Post tensioning)
Tendons
Icons on the vertical toolbar beside the tendon list are Add new tendon. After defining tendon properties and the tensioning process AxisVM determines the immediate losses of prestress and the equivalent loads for the end of tensioning (load case name-T0). Delete tendon. Deletes the selected tendon. Geometrical tansformations of tendons
Tendons selected in the tree can be translated or mirrored. Geometry for the new tendon can be defined using the toolbar beside the diagram.196
AxisVM 8+Release 4
4.10. Tendons can be copied or just moved.

Parameter values can be edited.
. After deleting the second base point the tendon geometry is deleted. and step 2. Select the postion of the cross-section where you want to define the tendom basepoint.
Rmin
To draw tendon geometry click the icons on the vertical toolbar beside the drawing and enter base points. Click the cable to add a new base point. Shows the precision of workmanship.User’s Manual
197
Parameters of the selected tendon appear beside the tendon list. You can close a tendon geometry with using Mouse Right Button/Complete. In case of several tendons this function only works with the active tendon. Following the first location repeat the step 1. The tendon position within the cross-section has to be specified only at the first base point. Ep Ap fpk µ k modulus of elasticity of tendon steel cross-section area of the tendon characteristic tensile strength of tendon steel coefficient of friction between the tendon and its duct (sleeve) unintentional angular displacement for internal tendons per unit length. to define all basepoint. Draw tendon in 2D.
Draw tendon in 3D. Add new base point. Delete base point. Initial values are 0°. For each basepoint the angles of tangent can be specified by setting the α (top view) and β (side view) values in the table.005 < k < 0. Select the postion of the cross-section where you want to define the tendom basepoint. Minimum radius of curvature. Double-click or Mouse Right Button/Complete to make the base point the last one. 2. Settle the tendon onto the proper position in the cross-section view. Enter values between -180° and 180°.01. The tendon position within the cross-section has to be specified at every basepoint. Clicking an existing base point deletes it. Further base points will be in the local x-z plane containing the first base point. AxisVM determines the trajectory passing through these base points as a cubic spline to minimize curvature. Following the first location you can position the other points of the tendon onto the longitudinal section. Ususally 0. Steps of drawing a tendon in 2D: 1. Base points can be created by clicking the diagram or using the coordinate window. In case of several tendons this function only works with the active tendon. Steps of drawing a tendon in 3D: 1. Where the radius of curvature is smaller than this limit tendons are displayed in red. You can position the tendon onto the top or at the bottom of the cross-section considering the concrete cover. Existing base points can be dragged to a new position using the mouse. Settle the tendon onto the proper position in the cross-section view. Position the tendon onto an optional point Position the tendon onto the neutral axis Position the tendon onto the top of the cross-section Position the tendon onto the bottom of the cross-section 2.

Possible operations and parameters: Tensioning from left / right / both side Release from left / right / both side Anchor on left / right / both side Force as a fraction of the characteristic value of tendon steel tensile strength (fpk ).14.
.
Options.198
AxisVM 8+Release 4
Table of base points
Base point properties can be edited in the table.1 Grid and Cursor Tensioning process The second tab is to define the tensioning process for tendons by determining the order of certain operations. Wedge draw-in of the anchorage device
Deletes the last operation from the list. Grid and cursor settings of the longitudinal and the cross-section diagram can be set. ecs(∞) is the long term value of the concrete shrinkage strain. Concrete The third tab is to check the material properties of the concrete.15. See… 2. Use the toolbar beside the table to add base points or remove the selected lines. Its value can be entered here.

A 2 (1 + c z cp ) [ 1 + 0 . If one tendon is selected in the tree two diagrams are shown. Long term loss of tension Long term loss of force due to shrinkage and creep of the concrete and the relaxation of the tendon is calculated as
ε cs E p + 0. Losses at anchorage are due to wedge draw-in of the anchorage devices.
where σmax Θ
is the maximum tension in the tendon is the sum of the absolute angular displacements over a distance x
2.  Ecm  where is the variation of stress at the centre of gravity of the cross-section ∆σc = (n–1) / 2n.
Immediate losses of tension 1. Tension loss due to friction between tendons and their ducts (sleeves) at position x measured from the anchorage point along the tendon is calculated as
σ µ ( x) = σ max (1 − e −µ(Θ + kx ) )
. If more than one tendon is selected the diagram shows the resultant equivalent load for the selected tendons only.User’s Manual
199
Results
If valid parameters.8ϕ Ac Ic
]
where ∆σc+s+r Ecm
is the tension loss due to the effects above is the secant modulus of elasticity of concrete
. Losses due to the instantaneous deformation of concrete are calculated as  j ∆σ c  ∆Pel = Ap Ep  . geometry and tensioning process is assigned to every tendon. result diagrams are displayed on the fourth tab. and the equivalent load for the tendon (F).QP
.8∆σ pr + ∆Pc + s + r = A p ∆σ c + s + r = A p 1+ Ep A p E cm Ep Ecm ϕ σ c . where n is the number of stressing steps j is the secant modulus of elasticity of concrete Ecm
∑
3. The first one is the actual tension along the tendon (fp /fpk).

98ρ1000 e8µ ⋅ 5000. due to selfweight and initial prestress and other quasi-permanent actions where relevant. The defined basepoints are always displayed in the Trajectory Table.
in case of 3rd relaxation class :
∆σ pr = σ max ⋅1.5% is the relaxation loss at a mean temperature of 20°C at 1000 hours after tensioning final value of creep coefficient is the stress in the concrete adjacent to the tendons. is the total cross-section area of tendons is the cross-section area of the concrete is the second moment area of the concrete section is the distance between the centre of gravity of the concrete section and the tendons
ϕ σc.1µ ⋅ 500 0 .QP
Ap Ac Ic zcp Trajectory table
The last tab is to build a trajectory table for the selected tendons with the desired increment and optional shift of origin.200
AxisVM 8+Release 4
∆σpr
is the long term absolute tension loss due to the relaxation of tendons in case of 2nd relaxation class :
∆σ pr = σ max ⋅ 0 .75 ( 1 − µ ) ⋅ 10 −5 .g.66 ρ1000 e 9.
Copy diagram
Ctrl+C
. Word).75(1− µ ) ⋅10−5
where ρ1000 = 2. This way the diagram can be pasted to other applications (e. Copies the drawing on the active tab to the Clipboard as a Windows metafile.
Main toolbar
The main toolbar has two buttons. The trajectory table consists of the local y and z coordinates of the selected tendons at the calculated x positions.

The joining works in case of single element../ Executes the command which was undone..User’s Manual
201
Print
Ctrl+P
Prints a report of the tensioning using diagrams and tables. Main toolbar / Copy diagram See. Main toolbar / Print
Undo/Redo Copy diagram Geometrical transformations of tendons Join connecting tendons
Undoes the effect of the previous command.. too.
Cross-sections can be selected to print cross-section diagrams.
. Tendons and report items can be selected.
Menu File Print Edit
You can reach the following functions via the menu:
See.. Tendons / Geometrical transformations of tendons
If more than one beam or rib element has been selected and these elements contain connecting tendons this function joins the connecting tendons... See. You can choose the position of the drawing (landscape or portrait) and set the scale of it (Print options for drawings).

Immediate mode
F
. load modification is similar to the load definition. If the Loads tab is active click a finite element to modify its loads.23. Modify
Modify
The nodal mass is displayed on the screen as two dark red concentric circles. Click the load type icon on the Toolbar. the loads due to the nodal masses are applied on the model. lines or surfaces.
4. If we select elements with loads not matching the load type we choose these loads remain unchanged. Close the dialog with OK. Enter new values. In fact. 3. If mass is the same in each direction it is enough to specify one value after checking Apply the same mass in each direction.. as well as the masses due to the applied loads. If the element has more than one load only one of them will come up. MZ . The display of this window can be turned on and off. 2. but does not assign loads to elements not being loaded and allows access to a specific load property without altering others. selection disappears and you can modify the element load you clicked. In second-order vibration analysis.
$
4. The display of this window can be turned on and off. Press the [Shift] key and select loads you want to modify (or the loaded elements).10. MY. 5.
To modify loads: 1. If more finite elements have been selected their loads can immediately be modified by clicking one of them.202
AxisVM 8+Release 4
Window
Coordinates Status
Editing of the longitudinal and cross-section diagrams is made easier by a coordinate window. If you have placed different concentrated and distributive loads on a beam and click the beam the load nearest to the click position will come up. If you click an element which is not selected.10. On diagrams an information window appears displaying diagram-specific information.22. Check the checkboxes beside the values you want to change. 4. You can also select by drawing a selection frame or using the Selection Toolbar. You can switch to the Define radio button to place loads on all the selected elements. Nodal Mass
In a vibration analysis the masses are concentrated at nodes that you can take into account by their global components MX.

4. 3..
Meshing of line elements Finite element analysis uses linear elements with constant cross-section so arced and variable cross-section (tapered) line elements must be divided into parts. This is called line element meshing. Maximum element size Length of the mesh lines cannot exceed the value specified.
. Removing a mesh does not delete loads and properties assigned to the line element.24.5 Delete
4. A mesh can also be defined for linear elements with constant cross-section. The accuracy of the solution depens on the mesh density. Mesh
Clicking the mesh tab mesh toolbar becomes available with mesh generation for line elements and domains.11. By angle Central angle of arced mesh segments cannot exceed the value specified. It is useful in nonlinear or vibration analysis when it is required to divide line elements to achieve a higher accuracy.1.User’s Manual
203
4. Division into N segments Line elements are divided into N parts.
4.10.2.11. mesh refinement functions and a finite element shape checking.11. Mesh Generation
Automatic detection of overlapping lines and missing intersections during meshing reduces the errors in model geometry.. Delete
[Del] See.
Mesh parameters for line elements
Mesh generation can be performed according to different criteria: Maximum deviation from arc Chord height cannot exceed the value specified.1. This mesh can be removed or modified just like a domain mesh.1.

Uniform mesh size Domain boundaries and inner lines will be divided according to the mesh size to ensure the given element size. Meshing will take into account all the holes. and disregards their corresponding line segments. If Create mesh only for unmeshed domains is checked no mesh will be created for domains already meshed. If there are existing quadrilateral or triangular meshes within the domain.2. The progress of the mesh generation process can be monitored in a window.1.
Mesh generation on domain A mesh of triangular surface elements can be generated on the selected domains by specifying an average surface element side length for the mesh.11. line loads will create mesh lines. The actual mesh can contain smaller and larger elements as well. Meshes will follow checked loads if load intensity exceeds the value specified.
The mesh generator uses only the end-points of beam elements that are in the plane of the domain. and can be canceled any time with the Abort button. and will integrate them in the new mesh.
Meshing paramaters for domains
Mesh size Fit mesh to loads Contour division method
An average mesh element size can be specified. the mesh generator will not change these meshes.204
AxisVM 8+Release 4
4. Rib elements are incorporated with their line segments because they can be defined on surface edges as well. Adaptive mesh size Adaptive meshing follows domain geometry and refine the mesh by reducing element size wherever it is necessary. Meshes can also follow loads above a certain intensity. the new mesh will replace the existing one.
Before Meshing
After Meshing
F
If a mesh is generated over an existing domain mesh (with a different average element side length). internal lines and points of the domain. Point loads will create mesh nodes.
.

You must specify the maximum side length of a surface element in the refined mesh.) as those in the coarse mesh.2. The elements in the refined mesh have the same properties (material. Mesh Refinement
Lets you refine the finite element mesh of surfaces.11. references.
Before mesh refinement
After mesh refinement
.User’s Manual
205
4.
Before mesh refinement
After mesh refinement
Bisection
Lets you refine the selected mesh by bisecting the elements as shown in the figure below
Quadrilateral element
Triangular element
Node relative
Lets you refine the mesh around the selected nodes (locally around columns. The following options are available:
Uniform
Lets you refine the entire selected mesh. nodal supports). etc.8).
F
You have to manually set the nodal degrees of freedom of the newly generated mesh that were not set automatically during the process of mesh generation. cross-section / thickness.2-0. The command refines the mesh dividing the elements connected to the respective nodes by the defined ratio. You must specify a division ratio (0.

2-0.
.8). Edge relative
Before mesh refinement
After mesh refinement
Lets you refine the mesh along the selected edges (locally along edge supports/loads). A triangular finite element is distorted if • 15. A qudrilateral finite element is distorted if • 30.11. You must specify a division ratio (0. You must specify a division ratio (0.2-0.3. nodal supports). Checking finite elements
Program checks the minimum angle of surface finite elements (α).206
AxisVM 8+Release 4
Lets you refine the mesh around the selected nodes (locally around columns. The command refines the mesh dividing the elements connected to the respective nodes by the defined ratio.
4. The command refines the mesh dividing the elements connected to the respective edges by the defined ratio.8).

The equilibrium equations in the direction of constrained degrees of freedom are not included in the system of equations. the results are displayed in the original node numbering. a node numbering optimization is performed in an iterative form to reduce the half-bandwidth of the system stiffness matrix. while the other displays the overall progress of the analysis process. vibration and buckling analysis.
Analysis
AxisVM lets you perform static.User’s Manual
207
5. The bar on the top displays the current step performed. AxisVM displays the evolution of the solution process by two progress bars. and details of the model can be displayed by pressing the Details button. Therefore to obtain support reactions you must model the support conditions using support elements. The node renumbering has effect only during the analysis process. not a replacement for engineering judgment. Note that the finite element analysis is only a tool.
Performing the analysis
. Model verification The input data is verified in the first step. The Cholesky method is applied to the solution of linear equilibrium equations.
Each analysis consists of three steps: 1) Model verification 2) Performing the analysis 3) Result file generation The actual running times of each step. Then. It implements an object-oriented architecture for the Finite Element Method. If an Error is found a warning message is displayed and you can then decide whether to cancel or continue the analysis. Press Esc key to skip this sequence. The instructions included in this User’s Manual assume a preliminary knowledge of the finite element method and experience in modeling. The eigenvalue problems are solved with the Subspace Iteration method.

internal force) is linearly related to the applied load.
Result file generation
5. it is assumed that the displacements remain within the limits of the small displacement theory. The term nonlinear means that the computed response (displacement. on how to use these elements in a linear analysis. beam. it is assumed that all materials and stiffness characteristics are linear-elastic.1. and spring elements in Chapter 4. rib and shell elements. Info palette shows this error as E(EQ). Through the geometric linearity. internal force) is nonlinearly related to the applied load. or taking into account the geometric nonlinearity of truss. If the value of E (Eq) is greater than 1E-06 the reliability of the computed results is questionable. Linear static Performs a linear static analysis.208
AxisVM 8+Release 4
Error of the solution
Solution error is calculated from the solution of a load case with a known result. In the following chapters we ‘ll show the setting of the parameters of the each calculation methods.
F
Nonlinear static
. See the description of the gap. that the Error of the displacements is of the same order. All the load cases are solved in the analysis. link or non-linear support. The materials assigned to surface elements can be othotropic. The term linear means that the computed response (displacement. It is a good estimation of the order of errors in displacement results for other load cases. Performs a nonlinear-elastic static analysis. This can be due to the use of gap. It is expected. truss or spring elements. Static Analysis
The term static means that the load does not vary or the variation with the time can be safely ignored. During the processing of the results the program sorts the results according to the original order of the nodes and prepares them to graphical display. Through the material linearity.

At least one criteria has to be selected. 0. Therefore it is important that the convergence tolerances to be set properly. E(U): relative error of the displacement convergence E(P): relative error of the force convergence E(W): relative error of the work convergence
. The default value is 1. AxisVM will perform nonlinear analysis for the selected load cases and shows a progress dialog. The criteria expressed in terms of work can be adequate for most problems. and work. However. During the iteration process.User’s Manual
209
Select load cases or combinations in the tree view.
Solution control Force When the Force control is selected.000001 for work. Load factor Load factor can be used to multiply loads of the selected load case or combination for the nonlinear analysis. AxisVM will determine if the nonlinear solution has reached the required accuracy (convergence). Convergence criteria Based on the convergence tolerances you specify. By default the value is set to 20. Number of increments Lets you specify the number of increments. Displacement/Load/Work/Convergence criteria In case of a nonlinear calculation you can specify multiple criteria. for monitoring the convergence of the nonlinear solution. Maximum iterations You can set the maximum number of the iterations based on the specifics of your model. you may specify a greater value in order to achieve convergence.001 for displacements. in terms of load. displacement. the norm of the unequilibrated load and/or of the iterational displacement increment vector must vanish (to approach zero). or vice-versa. no results will be obtained.001 for force. the increments are applied as equal fractions of the loads (as one parameter load). and 0. and of the incremental solution parameters. Displacement When displacement control is selected. Factors of convergence criteria has the following default values: 0. you may encounter a small Error in your unequilibrated load while the Error in displacements is still large. If the convergence is not achieved within the maximum number of iterations. When highly nonlinear behavior is analyzed. the increments are applied as equal fractions of the displacement component of the node specified. The relative errors at the end of the iteration process appear in the info window.

you may or may not include the geometrical nonlinearity for the above mentioned line elements (truss. the system stiffness matrix is updated only once. beam. in the first iteration of each increment. The method is known as the Modified Newton-Raphson technique. These results show the actual plate deflection and forces in the plate. AxisVM applies a Newton-Raphson iteration technique to the iterational solution of each increment. springs. The technique is known in different variants. rib and shell elements.
If n > MaxIterations. the system stiffness matrix is updated in each iteration.
. depending on the update of the system (stiffness) matrix. supports. The method is known as the classical Newton-Raphson technique. Displacements and internal forces of reinforced concrete plates are calculated according to the moment-curvature diagram of the reinforced cross-section of the plate.
Store last increment only Allows you to reduce the size of the results file when an incremental nonlinear analysis is performed with multiple increments (load or displacement) when just the results of the last increment are of interest to you.210
AxisVM 8+Release 4
Use reinforcement in calculation When analyzing reinforced concrete plates it is possible to take the